Download GSK218MC Series Machining CNC System Programming

This manual describes the various matters concerning the
operations of this CNC system as much as possible. However, it is
impossible to give detailed descriptions to all the unnecessary or
unallowable operations due to space limitation and product specific
applications. Therefore, the matters not specially described herein
should be considered as “impossible” or “unallowable”.
This user manual is the property of
GSK CNC Equipment
Co., Ltd. All rights are reserved. It is illegal for any organization or
individual to publish or reprint this manual. GSK CNC Equipment Co.,
Ltd. reserves the right to ascertain their legal liability.
This User Manual is suitable for the GSK CNC EQUIPMENT
CO., LTD.
GSK218MC Series Machining CNC System
Programming & Operation
The following CNC System are manufactured by GSK
Series
GSK218MC
Product Type
Structure
LCD Dimension
GSK218MC
Integral
10.4
GSK218MC-U1
Integral
8.4
GSK218MC-H
Horizontal
8.4
GSK218MC-H2
Horizontal
10.4
GSK218MC-V
Horizontal
10.4
Remark
LCD dimension is default
as 10.4 inch
LCD dimension is default
as 8.4 inch
LCD dimension is default
as 8.4 inch
LCD dimension is default
as 10.4 inch
LCD dimension is default
as 10.4 inch
Wherein, GSK218MC, GSK218MC-H and GSK218MC-V
are provided with three kinds of communication interfaces,
such as the RS232, USB and network, which are set at the
front face of the host.
GSK218MC-U1 owns only two communication interfaces,
such as the RS232 and USB, USB interface sets on the front
face of the host, and RS232 sets at the back of the host.
II
Security Warning & Precaution
III
GSK218MC Series Machining CNC System
Programming & Operation
PREFACE
Dear Users,
It is our pleasure for your patronage and purchase of this
machining center CNC system of GSK218MC series produced by
GSK CNC Equipment Co., Ltd.
This book is “Programming & Operation Manual”, which
introduces the programming and operation of the machining center
CNC system of GSK218MC series in detail.
To ensure the product works in a safe and efficient state, please
read this manual carefully before installation and operation.
SECURITY WARNING
Improper operations may cause unexpected accidents.
Only the person who owns the qualified professional can operate this
system.
Special prompt: The power supply fixed on/in the cabinet is exclusively
used for the CNC system made by GSK.
Never attempt to use this power as other purposes.
Otherwise, the enormous hazard may occur!
IV
Llist
SAFETY PRECAUTIONS
■ Transportation and storage
z
Do not pile up the packing boxes over 6 layers.
z
Never attempt to climb the packing box, neither stand on it, nor place heavy
objects on it.
z
Do not drag or move the products using the cables connected with the
product.
z
Avoid impact or scratch to the panel and screen.
z
Packing box should be protected from dampness, insolation and drench.
■ Open-package inspection
z
Confirm the product is the one you purchased after opening the package.
z
Check whether the product is damaged during transportation.
z
Confirm all the elements are complete without damage by referring to the list.
z
It is necessary to contact our company immediately if the product type is
inconsistent with the packing list, lack of accessories or damage in
transportation.
■ Wiring
z
Only the person who executes the wiring and inspection should have the
corresponding professional capacity.
z
The product should be reliably grounded, and its resistance should be less than
0.1Ω and can not be used the neutral conductor (zero cable) to replace the
ground wire.
z
The connection must be correct and secured. Otherwise, the product may be
damaged or unexpected results may occur.
z
The surge absorb diode connected with the product should be linked based
upon the described direction, otherwise, it may damage the product.
z
Turn off the power before inserting or unplugging a plug, or opening the electric
cabinet.
■ Overhaul
z
Turn off the power supply before troubleshooting or replacing components.
V
GSK218MC Series Machining CNC System
z
Programming & Operation
Overhaul the system when there is a short circuit or overload, and do not restart
it until the trouble is removed.
z Do not turn ON/OFF the product frequently, and the ON/OFF interval should be
1 minute at least.
DECLARTION
z We will try to describe all the various matters as much as possible in
this manual. However, it is impossible to give detailed descriptions to
all the unnecessary or unallowable operations because there are too
many possibilities. Therefore, the matters not specially described
herein should be considered as “impossible” or “unallowable”.
NOTICE
•
The functions and specifications (e.g., precision and speed)
described in this manual are only for this product itself. For those CNC
machine tools installing this product, the actual function configuration
and specifications depend on the designs of the machine tool
builders. Moreover, the function configuration and specifications of the
CNC machine tool are subject to the manual provided by the machine
tool builder.
All specifications and designs in this manual are subject to change without notice.
VI
Llist
BOOKⅠ
PROGRAMMING
This part introduces the technolog specification, production
types, command code and program format of the GSK218MC.
BOOKⅡ
OPERATION
This part introduces to the operation of the machining center
CNC system of GSK 218MC series.
APPENDIX
This part introduces the factory standard parameter and alarm
list, etc. of the machining center CNC system of the GSK218MC
series
VII
GSK218MC Series Machining CNC System
Programming & Operation
SECURITY RESPONSIBILITY
Security responsibility of the manufacturer
—— Manufacturer should take responsibility for the design and structure
danger of the CNC system and the accessories which have been eliminated
and/or controlled.
—— Manufacturer should take responsibility for the security of the CNC system
and accessories
—— Manufacturer should be take responsibility for the offered information and
suggestions for the user.
Security responsibility of the user
—— User should know and understand about the contents of security operation
by learning and training the CNC system safety operations.
—— User should take responsibility for the security and danger because of
increasing, changing or modifying the original CNC system and
accessories by themselves.
—— User should take responsibility for the danger without following the
operations, maintenance, installations and storages described in the
manual.
This manual is reserved by final user.
Sincere thanks for your support of GSK’s product!
Chinese version of all technical documents in Chinese and
English languages is regarded as final.
VIII
Llist
LIST
VOLUME I
PROGRAMMING ................................................................................................15
CHAPTER ONE
1.1
1.2
1.3
1.4
SUMMARY............................................................................................................ 1
Product Brief.............................................................................................................................................. 1
Technology Specification ......................................................................................................................... 2
Product Type Definition............................................................................................................................ 4
Bus Function Explanation........................................................................................................................ 5
CHAPTER TWO
PROGRAMMING BASIS ................................................................................... 7
2.1 Controllable axis ....................................................................................................................................... 7
2.2 Axis Name ................................................................................................................................................. 7
2.3 Axis Display ............................................................................................................................................... 7
2.4 Coordinate System................................................................................................................................... 8
2.4.1 Machine Tool Coordinate System......................................................................................................... 8
2.4.2 Reference Position................................................................................................................................ 8
2.4.3 Workpiece Coordinate System.............................................................................................................. 9
2.4.4 Absolute Coordinate Programming and Relative Coordinate Programming...................................... 10
2.5 Modal and One-shot............................................................................................................................... 11
CHAPTER THREE
COMPONENT PROGRAM CONFIGURATION ...................................... 13
3.1 Program Composition ............................................................................................................................ 13
3.1.1 Program Name.................................................................................................................................... 14
3.1.2 Sequency Number and Block ............................................................................................................. 14
3.1.3 Code Word .......................................................................................................................................... 14
3.2 General Structure of Program............................................................................................................... 18
3.2.1 Subprogram Compiling ...................................................................................................................... 19
3.2.2 Subprogram Calling............................................................................................................................ 20
3.2.3 Program End ....................................................................................................................................... 20
CHAPTER FOUR
PREPARATORY FUNCTION G CODE ........................................................ 21
4.1 Type of Preparatory Function G Code................................................................................................. 21
4.2 Simple G Code........................................................................................................................................ 26
4.2.1 Rapid Positioning G00........................................................................................................................ 26
4.2.2 Linear Interpolation G01 .................................................................................................................... 27
4.2.3 Circular Arc (Helical) interpolation G02/G03 .................................................................................... 28
4.2.4 Absolute/Incremental Programming G90/G91 ................................................................................... 34
4.2.5 Dwell (G04)........................................................................................................................................ 35
4.2.6 Single Direction Positioning (G60) .................................................................................................... 36
4.2.7 System Parameter On-Line Update .................................................................................................... 37
4.2.8 Workpiece Coordinate System G54～G59 ......................................................................................... 38
4.2.9 Additional Workpiece Coordinate System.......................................................................................... 41
4.2.10 Machine Coordinate System Selection G53 ..................................................................................... 41
4.2.11 Floating Coordinate System G92...................................................................................................... 42
4.2.12 Plane Selection G17/G18/G19.......................................................................................................... 44
4.2.13 Polar Coordinate Start/Cancel G16/G15........................................................................................... 44
4.2.14 Scaling Within Plane G51/G50......................................................................................................... 46
4.2.15 Coordinate System Rotation G68/G69 ............................................................................................. 50
4.2.16 Skip Function G31............................................................................................................................ 54
4.2.17 Inch/Metric Conversion (G20/G21).................................................................................................. 56
4.2.18 Optional Angle Chamfering/Corner Arc........................................................................................... 56
4.3 Reference Position G Code .................................................................................................................. 57
4.3.1 Reference Position Return (G28)........................................................................................................ 58
4.3.2 2nd, 3rd, and 4th Reference Position Retrun (G30) ............................................................................... 59
4.3.3 Automatically Return from Reference Position (G29) ....................................................................... 60
4.3.4 Reference Position Return Check (G27) ............................................................................................ 61
4.4 Canned Cycle G Code........................................................................................................................... 61
4.4.1 High-speed Peck Machining Cycle G73............................................................................................. 68
4.4.2 Drilling Cycle, Spot Drilling Cycle (G81).......................................................................................... 69
4.4.3 Drilling Cydle, Counter Boring Cycle (G82) ..................................................................................... 71
IX
GSK218MC Series Machining CNC System
Programming & Operation
4.4.4 Peck Drilling Cycle (G83).................................................................................................................. 73
4.4.5 Tapping Cycle G74 (or G84).............................................................................................................. 75
4.4.6 Fine Boring Cycle (G76).................................................................................................................... 79
4.4.7 Boring Cycle (G85)............................................................................................................................ 81
4.4.8 Boring Cycle (G85)............................................................................................................................ 82
4.4.9 Hole Cycle, Back Boring Cycle (G87)............................................................................................... 84
4.4.10 Boring Cycle (G88).......................................................................................................................... 86
4.4.11 Boring Cycle (G89) .......................................................................................................................... 88
4.5 Rigid Cycle G Code ............................................................................................................................... 90
4.5.1 Left-handed Rigid Tapping Cycle G74 .............................................................................................. 90
4.5.2 Right-handed Rigid Tapping G84....................................................................................................... 93
4.5.3 Peck Tapping (Chip-removal) Cycle .................................................................................................. 96
4.6 Compound Cycle G Code ................................................................................................................... 100
4.6.1 Groove Rough-Milling of Inner Circle (G22/G23) .......................................................................... 101
4.6.2 Fine-milling Cycle of the Full Incircle (G24/G25)........................................................................... 103
4.6.3 Excircle Fine-milling Cycle (G26/G32)........................................................................................... 105
4.6.4 Rectangular Groove Rough-milling (G33/G34)............................................................................... 107
4.6.5 Fine-milling Cycle within Rectangular Groove (G35/G36)............................................................. 109
4.6.6 Fine-milling ccle Outside the Rectangle (G37/G38) .........................................................................111
4.6.7 Canned Cycle Cancel (G80)................................................................................................................ 113
4.7 Tool Compensation G Code ............................................................................................................... 116
4.7.1 Tool Length Compensation G43, G44 and G49 ............................................................................... 116
4.7.2 Cutter Compensation G40/G41/G42 ................................................................................................ 119
4.7.3 Details of Cutter Compensation ....................................................................................................... 126
4.7.4 Corner Offset Arc Interpolation (G39) ............................................................................................. 143
4.7.5 Tool Compensation Value, Entering Compensation Number From Program (G10) ........................ 143
4.8 Feed G Code ........................................................................................................................................ 144
4.8.1 Feed Mode G64/G61/G63 ................................................................................................................ 144
4.8.2 Automatic Corner Override (G62) ................................................................................................... 145
4.9 Macro Function G Code ...................................................................................................................... 147
4.9.1 User Macro Program ........................................................................................................................ 147
4.9.2 Macro Variable ................................................................................................................................. 148
4.9.3 User Macro Program Call ................................................................................................................ 157
4.9.4 User Macro Program Function A ..................................................................................................... 157
4.9.5 User Macro Program Function B ..................................................................................................... 163
CHAPTER FIVE
MISCELLANEOUS FUNCTION M CODE.................................................. 171
5.1 M Code Control by PLC ...................................................................................................................... 172
5.1.1 Negative/Reverse Code Command (M03, M04).............................................................................. 172
5.1.2 Spindle Stopping Code Command M05........................................................................................... 172
5.1.3 Cooling ON/OFF (M08, M09) ......................................................................................................... 173
5.1.4 A Axis Releasing/Clamping (M10, M11)......................................................................................... 173
5.1.5 Tool Control Tool-releasing/Tool Clamping (M16, M17) ................................................................ 173
5.1.6 Spindle Orientation/Cancellation (M18, M19)................................................................................. 173
5.1.7 Tool-searching Code Command (M21, M22) .................................................................................. 173
5.1.8 Tool-magazine Return Code Command (M23, M24)....................................................................... 173
5.1.9 Rigid Tapping (M28, M29) .............................................................................................................. 173
5.1.10 Helical Chip-removal Conveyor ON/OFF (M35, M36)................................................................. 174
5.1.11 Punching Water Valve ON/OFF (M26, M27).................................................................................... 174
5.1.12 Spindle Blowing ON/OFF (M44, M45) ......................................................................................... 174
5.1.13 Automatic Tool-change Start/End (M50, M51).............................................................................. 174
5.2 M Codes for Controlling Program ...................................................................................................... 174
5.2.1 Program End and Return (M30, M02) ............................................................................................. 174
5.2.2 Program Dwell (M00) ...................................................................................................................... 175
5.2.3 Program Optional Dwell (M01) ....................................................................................................... 175
5.2.4 Program Calls Subprogram Code Command (M98) ........................................................................ 175
5.2.5 Program Ends and Rturns (M99)...................................................................................................... 175
CHAPTER SIX
SPINDLE FUNCTION S CODE........................................................................ 177
6.1 Spindle Analog Control ........................................................................................................................ 177
6.2 Spindle Switch Value Control.............................................................................................................. 177
6.3 Constant Surface Cutting Speed Control (G96/G97)...................................................................... 178
X
Llist
CHAPTER SEVEN
FEED FUNCTION F CODES ..................................................................... 183
7.1 Rapid Traverse...................................................................................................................................... 183
7.2 Cutting Speed........................................................................................................................................ 183
7.2.2 Feed per Revolution (G95) ............................................................................................................... 184
7.3 Tangential Speed Control .................................................................................................................... 185
7.4 Feedrate Override Button.................................................................................................................... 186
7.5 Automatic Acceleration/Deceleration................................................................................................. 186
7.6 Acceleration/Deceleration Treatment at Corner of Block................................................................ 187
CHAPTER EIGHT TOOL FUNCTION ....................................................................................... 189
8.1 Tool Function ......................................................................................................................................... 189
VOLUME TWO
CHAPTER ONE
OPERATION..............................................................................................191
OPERATION PANEL....................................................................................... 193
1.1 Panel Classification .............................................................................................................................. 193
1.2 Panel Function Explanation ................................................................................................................ 196
1.2.1 LCD Display Area ............................................................................................................................ 196
1.2.2 Editing Keyboard Area ..................................................................................................................... 197
1.2.3 Introduction of Screen Operation Buttons ........................................................................................ 199
1.2.4 GSK218MC Machine Tool Control Area ......................................................................................... 200
1.2.5 GSK218MC-H and GSK218MC-V Machine Tool Control Area ..................................................... 203
1.2.6 GSK218MC-U1 Machine Tool Control Area ................................................................................... 204
CHAPTER TWO
SYSTEM ON/OFF & SAFETY OPERATION.............................................. 207
2.1 System ON ............................................................................................................................................ 207
2.2 Power OFF ............................................................................................................................................ 207
2.3 Safety Operation................................................................................................................................... 208
2.3.1 Resetting Operation .......................................................................................................................... 208
2.3.2 ESP ................................................................................................................................................... 208
2.3.3 Feed Hold ......................................................................................................................................... 209
2.4 Cycle Start & Feed Hold ...................................................................................................................... 209
2.5 Overtravel Defense .............................................................................................................................. 210
2.5.1 Hardware Overtravel Defense .......................................................................................................... 210
2.5.2 Software Overtravel Defense............................................................................................................ 210
2.5.3 Releasing of Overtravel Alarm ......................................................................................................... 211
2.6 Stroke Inspection .................................................................................................................................. 211
CHAPTER THREE
INTERFACE DISPLAY & DATA MODIFICATION AND SETTING... 215
3.1 Position Display .................................................................................................................................... 215
3.1.1 Four Methods of Position Page Display ........................................................................................... 215
3.1.2 Display Machining Time, Component Numbers, Programming Speed, Override and Acutal Speed,
Etc. Information............................................................................................................................................ 217
3.1.3 Relative Coordinate Clear and Middle ............................................................................................. 219
3.1.4 Bus Monitoring Position Page Display............................................................................................. 220
3.2 Program Display ................................................................................................................................... 221
3.3 System Display ..................................................................................................................................... 225
3.3.1 Display, Modification and Setting of Offset ..................................................................................... 225
3.3.1.1 Display of Offset..................................................................................................................... 225
3.3.1.2 Modification and Setting of Offset Value ............................................................................ 227
3.3.2 Display, Modification and Setting of Parameter............................................................................... 227
3.3.2.1 Parameter Display ................................................................................................................. 227
3.3.2.2 Modification and Setting of Parameter Value .................................................................... 229
3.3.3 Display, Modification and Setting of Macro Variable ...................................................................... 229
3.3.3.1 Display of Macro Variable..................................................................................................... 229
3.3.3.2 Modification and Setting of Macro Variable ....................................................................... 231
3.3.4 Display, Modification and Setting of Ptich Compensation............................................................... 231
3.3.4.1 Pitch Compensation Display ................................................................................................ 231
3.3.4.2 Modification and Setting of Pitch Compensation .............................................................. 232
3.3.5 Display, Modification and Settong of Bus Servo Parameter............................................................. 232
3.3.5.1 Servo Parameter Display...................................................................................................... 234
3.3.5.2 Spindle Parameter ................................................................................................................. 237
3.3.5.3 Servo Debugging Tool STT .................................................................................................. 240
XI
GSK218MC Series Machining CNC System
Programming & Operation
3.3.5.4 Double-drive Debugging Tool .............................................................................................. 245
3.4 Setting Display...................................................................................................................................... 247
3.4.1 Setting Page...................................................................................................................................... 247
3.4.2 Workpiece Coordinate Setting Page ................................................................................................. 249
3.4.3 Center and Tool-setting Function ..................................................................................................... 250
3.4.3.1 Center Function Introduction & Operation Explanation ................................................... 251
3.4.3.2 Introduction and Operation Explanation of Tool-setting Function .................................. 257
3.4.4 Backup, Recovery and Transmission of Data................................................................................... 260
3.4.5 Setting & Modification of Password Authority................................................................................ 264
3.5 Figure Display....................................................................................................................................... 265
3.6 Diagnosis Display................................................................................................................................. 267
3.6.1 Diagnosis Data Display.................................................................................................................... 268
3.6.1.1 Signal Parameter Display .................................................................................................... 268
3.6.1.2 System Parameter Display .................................................................................................. 270
3.6.1.3 Bus Parameter Display......................................................................................................... 270
3.6.1.4 DSP Parameter Display ....................................................................................................... 271
3.6.1.5 Fluctuation Parameter Display ............................................................................................ 271
3.6.2 Check Signal State ........................................................................................................................... 272
3.7 Alarm Display........................................................................................................................................ 272
3.8 Program-Control Display..................................................................................................................... 275
3.9 Help Display.......................................................................................................................................... 277
CHAPTER FOUR
MANUAL OPERATION................................................................................ 285
4.1 Coordinate Axis Movement................................................................................................................. 285
4.1.1 Manual Feed..................................................................................................................................... 285
4.1.2 Manual Rapid Traverse .................................................................................................................... 285
4.1.3 Manual Feed & Manual Rapid Traverse Rate Selection .................................................................. 285
4.1.4 Manual Intervention ......................................................................................................................... 286
4.1.5 Workpiece Correction....................................................................................................................... 287
4.2 Spindle Control ..................................................................................................................................... 289
4.2.1 Spindle Positive................................................................................................................................ 289
4.2.2 Spindle Negative .............................................................................................................................. 289
4.2.3 Spindle Stop ..................................................................................................................................... 289
4.2.4 Automatic Shift of Spindle............................................................................................................... 289
4.3 Other Manual Operations.................................................................................................................... 290
4.3.1 Coolant Control................................................................................................................................ 290
4.3.2 Lubrication Control .......................................................................................................................... 290
4.3.3 Chip-removal Control ...................................................................................................................... 290
4.3.4 Workping Indicator Control............................................................................................................. 291
CHAPTER FIVE
SINGLE-STEP OPERATION ......................................................................... 293
5.1 Single-step feed.................................................................................................................................... 293
5.1.1 Movement Amount Selection........................................................................................................... 293
5.1.2 Selection of Movement axis and Movement Direction .................................................................... 294
5.1.3 Single-step Feed Explanations ......................................................................................................... 294
5.2 Single-step Interruption ....................................................................................................................... 294
5.3 Auxiliary Control in Single-step Operation........................................................................................ 294
CHAPTER SIX
MPG OPERATION ............................................................................................. 295
6.1 MPG Feed ............................................................................................................................................. 295
6.1.1 Selection of Movement Amount....................................................................................................... 295
6.1.2 Selection of Movement Axis and Direction ..................................................................................... 296
6.1.3 MPG Feed Explanations................................................................................................................... 296
6.2 Control for MPG Interruption Operation............................................................................................ 296
6.2.1 Operation of MPG Interruption........................................................................................................ 296
6.2.2 Relationships Between MPG Interruption and Other Fucntions ...................................................... 298
6.3 Auxiliary Control During MPG Operation.......................................................................................... 298
6.4 Electric MPG Drive Function .............................................................................................................. 298
CHAPTER SEVEN
AUTOMATIC OPERATION....................................................................... 299
7.1 Selection of Auto Operation................................................................................................................ 299
7.2 Start of Auto Operation ........................................................................................................................ 299
7.3 Stop of Auto Operation ........................................................................................................................ 300
XII
Llist
7.5 Dry Run .................................................................................................................................................. 302
7.6 Single Block Operation ........................................................................................................................ 302
7.7 Machine Locking Operation ................................................................................................................ 302
7.8 M.S.T Function Locking Operation .................................................................................................... 303
7.9 Feed, Rapid Trimming in Auto Operation.......................................................................................... 303
7.10. Spindle Speed Trimming in Auto Mode .......................................................................................... 304
7.11 Background Editing in Auto Mode .................................................................................................... 305
CHAPTER EIGHT MDI OPERATION........................................................................................ 307
8.1
8.2
8.3
8.4
MDI Code Input..................................................................................................................................... 307
Operation and Stop of MDI Code Block ............................................................................................ 308
Modification and Clear of Filed Value in MDI Code Block .............................................................. 308
Conversion of Each Operation Mode ................................................................................................ 308
CHAPTER NINE
ZERO RETURN OPERATION.......................................................................311
9.1 Concept of Machine Tool Zero (Mechanical Zero)........................................................................... 311
9.2 Operation Steps for Pulse Servo Mechanical Zero Return ............................................................ 311
9.3 Operation Steps for Mechanical Zero Return Specified by Program ............................................ 312
9.4 Bus Servo Zero-Return Function Setting .......................................................................................... 312
9.4.1 Common Zero Turn .......................................................................................................................... 313
9.4.2 High Speed Increment Zero Return .................................................................................................. 313
9.4.3 Multi-Core Absolute Zero Setting .................................................................................................... 314
CHAPTER TEN
EDIT OPERATION........................................................................................... 317
10.1 Edit of Program................................................................................................................................... 317
10.1.1 Establishment of Program............................................................................................................... 318
10.1.1.1 Automatic Generation of Sequence Number .................................................................. 318
10.1.1.2 Input of Program Content................................................................................................... 318
10.1.1.3 Index of Sequence Number, Word and Line Number .................................................... 320
10.1.1.4 Positioning method of cursor ............................................................................................. 321
10.1.1.5 Insertion, Deletion and Modification of Word .................................................................. 322
10.1.1.6 Deletion of Single Block ..................................................................................................... 322
10.1.1.7 Deletion of Multi-Block ........................................................................................................ 323
10.1.1.8 Deletion of Multiple Code Word......................................................................................... 323
10.1.2 Deletion of Single Block ................................................................................................................ 324
10.1.3 Deletion of Overall Programs ......................................................................................................... 325
10.1.4 Program Copy................................................................................................................................. 325
10.1.5 Copy and Paste of Block................................................................................................................. 325
10.1.6 Cut and Paste of Block ................................................................................................................... 326
10.1.7 Replacement of Block..................................................................................................................... 327
10.1.8 Rename of Program ........................................................................................................................ 327
10.1.9 Program Restart .............................................................................................................................. 327
10.2 Program Administration ..................................................................................................................... 329
10.2.1 Index of Program List..................................................................................................................... 329
10.2.2 Quatity of Storage Program ............................................................................................................ 330
10.2.3 Storage Capacity............................................................................................................................. 330
10.2.4 Check of Program List.................................................................................................................... 330
10.2.5 Locking of Program........................................................................................................................ 330
CHAPTER ELEVEN
SYSTEM COMMUNICATION ............................................................... 331
11.1 Serial Port Communication ............................................................................................................... 331
11.1.1 Program Start .................................................................................................................................. 331
11.1.2 Function Introduction ..................................................................................................................... 332
11.1.3 Series Port Data Transmission ........................................................................................................ 333
11.1.4 Series Port DNC ON-Line Machining ............................................................................................ 336
11.2 USB Communication.......................................................................................................................... 338
11.2.1 Brief & Precaution .......................................................................................................................... 338
11.2.2 USB Component Program Operation Steps.................................................................................... 339
11.2.3 USB DNC Machine Operation Steps........................................................................................... 341
11.2.4 Retreat from U Disk Operation Interface........................................................................................ 342
APPENDIX ................................................................................................................................343
APPENDIX ONE
GSK218MC SERIES PARAMETER LIST ................................................... 345
XIII
GSK218MC Series Machining CNC System
Programming & Operation
Parameter Explanation ................................................................................................................................. 345
1. Bit Parameter............................................................................................................................................ 346
2. Data Parameter ......................................................................................................................................... 368
Appendix Two
XIV
Alarm List............................................................................................................... 409
VOLUME I
PROGRAMMING
VOLUME I PROGRAMMING
XIX
GSK218MC Series Machining CNC System
VOLUME I
PROGRAMMING
XVIII
Programming & Operation Manual
Chapter One
Summary
CHAPTER ONE
1.1
SUMMARY
Product Brief
GSK218MC Series Machining Center CNC System is a kind of upgraded product of
GSK218M, which uses the high-velocity spline interpolation calculation; the machining
velocity, accuracy and the fineness of the surface are greatly enhanced accordingly; the
newly designed man-machine interface is more beatiful, friendly and useful, which
supports the GSK-LINK Ethernet bus function, and the connection is more convenient;
briefer. It can be adapted with the Milling Machine Center, High velocity CNC engraving
and milling machine, grinding machine and hobbing machine, etc.
z
High velocity & high accuracy, complicated curve surface machining efficient velocity
8m/min, optimal machining velocity 4m/min.
z
Top position velocity 60m/min, the Max. feedrate150m/min.
z
Up to 1000 for the pretreatment sections, it owns the prospect function, high velocity,
high accuracy and good smoothness.
z
The installation structure divides into integral, horizontal and vertical, which is
1
VOLUME I
PROGRAMMING
as well, it supplies the statement macro program (Macro B), so that the programming is
GSK218MC Series Machining CNC System
Programming & Operation Manual
separately used the 8.4/10.4 inch high resolution color LCD.
z
the newly designed man-machine interface is more beatiful, friendly and useful.
z
It supports the Chinese, English, Russian, Spanish and Turkey, etc.
z
It supports the functions, such as the PLC on-line monitoring, editing, compiling and
signal trace.
z
It supports many kinds of tool magazines, for example, the turntable, disk and servo
one.
z
It supports the statement macro program (Macro B)
z
Abundant help, prompt information; and easy to learn, use and debugging.
z
It spports the RS232, USB and network 3-kind communication interfaces, which
VOLUME I
PROGRAMMING
carries out the file transmission, DNC machining, USB on-line machining.
z
It supports the GSK-LINK Ethernet bus function for convenient connection and
strong extension, and supports the 17-bit absolute encoder with high accuracy,
against to zero return, which can be carried out the full-closed-loop control
(Optional).
1.2
Technology Specification
Controllable axis and linkage axis: the standard configuration is 4-axis
Movement control
3-linkage; the 4-axis 4-linkage can be matched. Each axis can be regarded as
linear axis or rotation one.
Interpolation method: Positioning (G00), straight line (G01), circular arc (G02,
G03) and helix interpolation.
Position command range: Metric: -99999.999mm～99999.999mm, the least
command unit: 0.001mm;
Inch: -9999.9999inch ～ 9999.9999inch, the least
command unit 0.0001inch;
Electric gear: Command multiplication coefficient 1 ～ 65536, command
frequency-devision coefficient 1～65536.
Rapid traverse rate: Up to 60m/min, rapid override: F0, 25％, 50％ and 100％
4-level real-time adjustment.
Cutting feedrate: Up to 15m/min (G94) or 500.00mm/r (G95)
Feedrate: 0 ～ 200 ％ 21-level real-time adjustment, wave-section control
available;
2
Chapter One
Summary
MPG feed: 3-gear (0.001, 0.01 and 0.1mm); single feed: 4-gear (0.001, 0.01,
0.1 and 1mm)
Forward acceleration: The linear acceleration/deceleration or S-type one can
be selected; the acceleration/deceleration time constant can be set.
Acceleration/
deceleration
Backward deceleration: The linear acceleration/deceleration or index one can
be alternative; the acceleration/deceleration time constant can be set.
Wherein, Manual, MPG and single step are used the backward deceleration.
The rapid positioning, cutting feed can be selected the forward/backward
acceleration or deceleration.
It is specified by M and 2-digit; M function can be self-defined.
System internal M command (do not repeatedly define): End-of-program M02,
function
Tool function
M30; Program stop M00; Optional stop M01, Tool-magazine call M06,
Subprogram call M98 and Subprogram end M99;
The defined M commands by PLC: M03, M04, M05, M08, M09, M10, M11, M16,
M17、M18, M19, M20, M21, M22, M23, M2, M26, M27, M28, M29, M35, M36,
M44, M45, M50 and M51
Tool function
● T and 4-digit tool selection ●256 groups tool offset value ● length
compensation ● worn compensation ●C-type Cutter comensation
● S2 digit (I/O gear control) /S5 digit (Analog output) ● Top spindle velocity limit
● Constant line velocity function;
Spindle encoder: The encoder linear number can be set to (100～5000p/r); the
Spindle function
driving ratio between encoder and spindle: (1～255) : (1～255);
Spindle override: 50%~120% 8-level real-time adjustment in total, which can be
performed the wave-band control.
Tapping cycle, flexible tapping and rigid tapping
● Pitch error compensation: Compensation interval, compensation origin can
be set, compensation value range: -999 ~ +999 pulse equivalent.
● Reverse interval compensation: The reverse interval value can be
Automatic
compensation
compensated by setting the fixed frequency or lifting method.
● Cutter length compensation: A or B type length compensation function can be
selected by parameter.
● Cutter raidus compensation: C-cutter compensation function, the Max.
compensation value is ±999.999mm or ±99.9999inch
Reliability and
safety
State signal: ●ESP ●Overtravel ●Stored stroke limit ●NC ready signal ●Servo
ready signal ●MST function completion signal ●Auto operation start indicator
signal ●Auto operation signal during motion ●Feed hold indicator signal
Self-diagnosis
function:
●Signal
●System
●Position
control
●Servo
●Communication ●Spindle
3
VOLUME I
PROGRAMMING
Miscellaneuos
GSK218MC Series Machining CNC System
Programming & Operation Manual
NC alarm: ●Program ●Operation ●Overtravel ●Servo ●Connection ●PLC
●Memory (ROM and RAM)
●Edit ●Auto ●MDI ●Zero return ●Manual ●Single step ●DNC ●Single block
Operation
●Skip ●Dry run ●M.S.T lock ●Program restart ●MPG interrupted ●Single step
function
interrupted ●Manual interference ●Machine lock ●Interlocking ●Feed hold
●Cycle start ●ESP ●External reset signal ●External power ON/OFF
●GSK 218MC, GSK 218MC-V system uses the color 10.4 inch LCD with the
resolution 800×600.
●GSK 218MC-H, GSK 218MC-U1 system uses the color 8.4 inch LCD with the
resolution 800×600.
VOLUME I
PROGRAMMING
Display
●It provides 5 kinds of interfaces, such as the Chinese, English, Russian,
Spanish and Turkey, which can be selected by parameter.
●Position information ●User program ●System setting ●PLC ●Diagnosis
parameter ●Figure ●Alarm information ●Help
●Actual feedrate, spindle speed ●Real-time wave diagnosis ●System operation
time (NC command and state information)
Program capacity: 57M, up to 400 programs can be stored.
Program edit
●Program preview ●Program edit ●Backstage edit;
PLC treatment velocity: 3us/step; up to 4700 steps; basis command 10 pieces,
35 function commands; ladder diagram on-line edit;
PLC Function
IO unit input/output: 48/48, extendible;
Communication
function
Adapted drive
1.3
4
Support the RS-232 series port, USB, network communication interface, file
transportation available, DNC machining function (series port, network) and
USB on-line machining function
DA98 Series, GS Series, GE Series Digit AC Servo, etc.
Product Type Definition
GSK218
M
1
2
( C ) ( a )
3
4
( H )
( 1 ) ( 1 )
5
6
Chapter One
Series
Summary
Code Explanation
No.
Product type main character part: GSK218 series
①
Function (Machining object) configuration: It expresses by Capital English Letters.
②
M - Milling machine
Series continuation: It is indicated by Capital English Letters. Without: Initial version
③
Sub-series continuation (or improvemen number): It expresses by Lowercase English
④
Letters, such as a, b, c…. Without: Initial version
Structure
dedicated
Structure type: It separately expresses by Capital Letters U, H, V and B.
U-Integral,
H-Horizontal,
V-Vertical,
B-Cabinet.
VOLUME I
PROGRAMMING
⑤
or
type
type
Dedicated type: It expresses by Capital Letter P.
LCD dimension LEC dimension: It expresses by one number (1～9).
(structure)
⑥
or 1: 8.4 inch, 2: 10.4 inch, 3～9: …,
dedicated code
Dedicated type: It expresses by two numbers (01～99).
Example
◆ GSK218MC-H: 218MC Series, Horizontal structure, 8.4 inch LCD (Defualt
dimension)
◆ GSK218MC-H2: 218MC Series, Horizontal structure, 10.4 inch LCD
◆ GSK218MC-U1: 218MC Series, Integral structure, 8.4 inch LCD
◆ GSK218MC-P01: 218MC Series, No.01 dedicated machine
◆ GSK218MCa-P25: 218MCa Series, No.25 dedicated machine
1.4
Bus Function Explanation
This system adds Ethernet Bus Communication method from the beginning of the system
software version V1.4.
The functions described in this manual are suitable for the Bus and Pulse transmission methods.
For the former, the new addition function for this system will particularly explain.
Refer to the following description when selecting the Ethernet Bus Communication Method or
Pulse Communication Method.
Method one:
5
GSK218MC Series Machining CNC System
Programming & Operation Manual
1. Enter the <MDI> operation method;
2. Enter the <SET> page by
, then enter the password page by [PASSWORD], input the
corresponding level password; refer to the Section 3.4.5
Authorization Book II
Setting and Modification of Password
OPERATION in this manual;
3. Set the parameter switch to “1” in the <SETTING> interface;
4. Enter into to the page to perform the seting together by the
, then the [
Bus
Configuration] (Refer to the Fig. 1-4-1):
1) Move the cursor to the item of the “Bus or not”;
VOLUME I
PROGRAMMING
2) Input the “1”, select the Bus; or input the “01”, select the pulse;
Fig. 1-4-1
Mehtod 2:
The drive transmission method is Bus by directly setting the bit parameter No: 0#0=1; it is the
pulse by setting the No: 0#0=0
Note: It is necessary to cut off the overall powers before modifying this parameter; turn on the power again
after performing it.
6
Chapter Two Programming Basis
CHAPTER TWO
2.1
PROGRAMMING BASIS
Controllable axis
Table 2-1-1
Item
GSK218MC
Basis controllable axis number
3 axes (X, Y and Z)
Extension controllable axis number
Up to 5 axes
Occasionally, there is not alternative other than to use a additional axis because the structure
design requirement for some machine tools, such as the revolving worktable, rotation worktable, etc.
This axis can be set as both linear axis and rotation axis. GSK218MC can be set each axis as linear
oen or rotation one.
2.2 Axis Name
The names of the 3 basic axes are X, Y, Z and A by default.
The number of the controlled axes is set by data parameter P005, and the name of each
additional axis, such as A, B and C, is set by P175-P179.
Note: If the inputted axis name is repeated, the system may automatically initialize as X, Y, Z, A and B.
2.3
Axis Display
When the additional axis is set as rotation one, and the unit of the rotation axis displays as deg; if
it is set as linear one, the display is identical with the basis 3 axes (X, Y and Z), and its unit is mm.
The following figure shows that the 4th axis is regarded as the linear one, and the 5th is treated as the
rotation one.
7
VOLUME I
PROGRAMMING
(total)
GSK218MC Series Machining CNC System
Programming & Operation Manual
VOLUME I
PROGRAMMING
Fig. 2-3-1
2.4
Coordinate System
2.4.1
Machine Tool Coordinate System
A special point on a machine used as machine benchmark is called machine zero, which is set
by the machine tool builder. The coordinate system with machine zero point set as its origin is called
the machine coordinate system. It is set up by manual machine zero return after the power is turned
on. Once set, it remains unchanged till the power off, system reset or emergency stop.
A special point on a machine used as machine benchmark is called machine zero, which is set
by the machine tool builder. The coordinate system with machine zero point set as its origin is called
the machine coordinate system. It is set up by manual machine zero return after the power is turned
on. Once set, it remains unchanged till the power off, system reset or emergency stop.
2.4.2
Reference Position
There is a special point on the CNC machine tool for tool change and coordinate system setup.
This point is called reference point. It is a fixed point in the machine coordinate system set by the
machine tool builder. By using reference point return, the tool can easily move to this position.
Generally this point in CNC milling system coincides with the machine zero, while it is usually the tool
change point for machining center.
8
Chapter Two Programming Basis
Reference position
Tool
Workpiece
Worktable
Fig. 2-4-2-1
VOLUME I
PROGRAMMING
There are two methods to move the tool to the reference point:
1.
Manual reference position return (Refer to the Chapter Nine
2.
Auto reference point return
2.4.3
Zero Operation)
Workpiece Coordinate System
The coordinate system used for workpiece machining is called workpiece coordinate system (or
part coordinate system), which is preset by CNC system (set in workpiece coordinate system setting).
Tool
Z
Y
Z
Z
Y
Program
X
Machining drawing
X
Command
Coordinate system
Y
X
CNC system
Machine tool
Fig. 2-4-3-1
In the coordinate system specified by CNC, in order to cut the workpiece into the shape on the
drawing according to the program of the programming coordinate system on the drawing, the
relationship between machine tool coordinate system and workpiece coordinate system must be
determined. The method to determine the relationship between these two coordinate systems is
called alignment. It can be done by different methods depending on part figure, workpiece quantity,
etc.
9
GSK218MC Series Machining CNC System
I) The reference point with component
Programming & Operation Manual
II) Install the component on the fixture directly
Reference point
Workpiece
fixture
Workpiece
reference position
Fixed
distance
The tool should be positioned at the specified
distance (it can be a reference point) from the
reference position, because the tool center can
not directly located at the workpiece point. Set
the workpiece coordinate system specified by
CNC using the specified distance. (For
example: G92)
Tool center movement aims at the
component reference position, set the
workpiece coordinate system by CNC
command at this place; in this case, the
workpiece coordinate system is overlapped
with the one of the programming.
Fig. 2-4-3-2
VOLUME I
PROGRAMMING
A machining program sets a workpiece coordinate system (selecting a workpiece coordinate
system). The workpiece coordinate system set can be changed by moving its origin.
There are two methods to set the workpiece coordinate system:
1. Using G92, see 4.2.11 for details.
2. Using G54-G59, see 4.2.8 for details.
2.4.4
Absolute Coordinate Programming and Relative Coordinate
Programming
There are absolute and relative definitions to define the axis moving amount. The absolute
definition is a method to program by the coordinate of the end point of the axis movement, which is
called absolute programming. Relative definition is method to program directly by the axis moving
amount, which is call relative programming (also called incremental programming).
1) Absolute coordinate value
It is the target position coordinate in the specified workpiece coordinate system, namely, the
position to which the tool is moved.
Z
A(15,60,40)
B (10,30,20)
Y
X
Fig. 2-4-4-1
10
Chapter Two Programming Basis
G90 G54X10 Y30 Z20;
Move the tool from point A to point B using the point B coordinate in G54 workpiece coordinate
system. The instruction is as follows:
2) Incremental coordinate value
It is the target position coordinate relative to the current position with the current position set
as the origin.
Cutter
Z
A
30
10
VOLUME I
PROGRAMMING
40
B
Y
X
Fig. 2-4-4-2
Tool rapidly moves to the point B from A, its code as follows:
G0 G91 X40 Y-30 Z-10；
2.5
Modal and One-shot
Modal, that of the value of one address, will keep enabling as soon as setting, until this address
is reset again. The another meaning of the modal is that this field may not input if the same function is
used in the following block after one function word is set.
¾
For example:
G0 X100 Y100;
X20 Y30；
(Rapid positioning to X100 Y100)
(Rapid positioning to X20 Y30，G0 is modal, which can be ignored.)
G1 X50 Y50 F300; (Linear interpolation to X50 Y50，feedrate 300mm/min G0→G1)
X100；
(Linear interpolation to X100 Y50，feedrate 300mm/min，G1, Y50 and
F300 are the modal, which can be ignored.)
G0 X0 Y0；
(Rapid positioning to X0 Y0)
The initialized state is the default one after the system is turned on. Refer to the table 4-1-2.
¾
For example:
O00001
11
GSK218MC Series Machining CNC System
Programming & Operation Manual
X100 Y100；（Rapd positioning to X100 Y100，G0 is the system iniliatization）
G1 X0 Y0 F100；（Linear interpolation to X0 Y0, feed/min., feedrate is 100mm/min）
One-shot, the corresponding address value, is only enabled in the block written this code; if this
address value is used again in the next block which should be specified it again. Refer to the G
function code in the group 00 in table 4-1-2.
The modal and one-shot descriptions of the function words are refer to the table 2-5-1
Table 2-5-1
Modal and one-shot of function code
A group of G functions can be cancelled each other.
Modal G
These functions will always enable once they are
function
performed until cancelled by a same group G
VOLUME I
PROGRAMMING
functions.
Modal
Modal M
function
One-shot G
One-shot
function
One-shot M
function
12
A group of M functions can be cancelled each other,
which keeps enabling before canceling by another
function in the same group.
It is only enabled in the specified block, which is
cancelled when the block ends.
It is only enabled in the block of writing this code.
Chapter Three
CHAPTER THREE
3.1
Component Program Configuration
COMPONENT PROGRAM CONFIGURATION
Program Composition
A program composes of doubles of blocks; a block consists of words. Each block is divided into
by EOB code (ISO is LF; EIA is CR). The character “;” described in this manaual means the code of
EOB.
VOLUME I
PROGRAMMING
Fig. 3-1-1
Program structure
The code series collection for controlling CNC machine tool to perform the component machining
is regarded as program. After the written program is input to the CNC system, the system can be
moved the tool along with the straight line, arc or performed the rotation and stop to the spindle based
upon the codes. In program, these codes will be compiled according to the actual movement
sequence of the machine tool. The program structure is as Fig. 3-1-1.
13
GSK218MC Series Machining CNC System
3.1.1
Programming & Operation Manual
Program Name
The system memory can be registered several programs. At the beginning of the program, in
order to distinguish from these programs, the address O and its following 5-digit is treated as program
name, refer to the Fig. 3-1-1-1.
O
Program No. (0~99999，the leading zero can
be omitted when it is input.)
Address O
Fig. 3-1-1-1 The composition of program name
VOLUME I
PROGRAMMING
3.1.2
Sequency Number and Block
Program consists of multiple codes, one of the code unit is regarded as the block (Refer to the
Fig. 3-1-1). Program end codes are divided into the blocks (Rerfer to the Fig. 3-1-1). The EOB code
will show by the character “;” in this manual.
The sequence number (Refer to the Fig. 3-1-1) constituted with the address N and its following 4
numbers can be used at the beginning of the block, the front code leading-zero can be omitted. The
order of the sequence number is arbitary (Whether to insert the sequence number is set by bit
parameter NO:0 # 5, or directly set in the setting interface, refer to the Section 3.4.1 in the
OPERATION); its intervals can be set as in variety (the interval size is determined by parameter
P210). Also, the sequence number can be specified for either the overall blocks or the important
blocks. Generally, the machining sequence is increasing gradually. It is for the convient that the
sequence numbers are specified at the important position (For example, tool-change or the worktable
index moves to the new machining interface, etc.)
Note: N code is not regarded as the line number whe it is shared a same block with the G10.
3.1.3
Code Word
Code word (Fig. 3-1-3-1) is the essential factor for composing the block, which is cosists of the
address and its following numbers (sometimes, the +/- symbol may specify in front of the number).
X
100
Add. No.
Code word
Fig. 3-1-3-1
14
the composition of the code word
Chapter Three
Component Program Configuration
The address is one of the English letters (A~Z), which specifies the meaning of its following
numerical value. In this system, the usable address and its meaning, as well the resolution range are
as the Fig. 3-1-3-1.
Occasionally, one address owns different meanings based upon the variable preparation
functions.
If two or more same addresses are displayed at a same code, which is determined by bit
parameter No: 32#6 to alarm or not.
Table 3-1-3-1
Add.
Resolution range
Function meaning
A, B, C
It is set by data parameters
Axle name address
VOLUME I
PROGRAMMING
P175~179
Radius offset number, D0 is regarded as
D
0～255
0 by default; user can neither set nor
modify it.
E
Not use yet
F
0.001～99999.999（mm/min）
Feedrate/min.
0.001～500(mm/r)
Feedrate/rev.
G
00～99
Preparation function
01～99
Calculation symbol in G65
Length offset number, H0 is treated as 0
H
0～255
by default; User can neither set nor
modify it.
The relative start of circular center is at
I
-99999999～99999999（mm）
the X axis vector (Circular arc/helix
interpolation, zoom in/out)
I shouls be more than the current
tool radius
(Cutter
radius
<I≤99999.999mm,
+
it
is
G22/G23 groove radius inside circle
J)
the
absolute value when in the
G24/G25, G26/G32 finish-milling radius
of the circle
negative.
I
>
{(Data
parameter
P269
setting value * cutter radius) +
cutter radius}*2.
Cutter radius under the helix <
Width of G33/G34 rectangle groove
along with the X axis direction
{( I/2) – cutter radius}
15
GSK218MC Series Machining CNC System
Add.
Resolution range
0<I≤99999.999mm,
it
Programming & Operation Manual
Function meaning
is
the
absolute value when in the
negative.
Width of G35/G36, G37/G38 rectangle
groove along with the X axis direction
The vectior of the circular arc center
-99999999～99999999（mm）
relative start along with the Y axis
(Arc/helix interpolation and scaling)
0≤J≤99999.999mm,
VOLUME I
PROGRAMMING
J
it
is
the
The circle center distance between
absolute value when in the
G24/G25, G26/G32 finish-milling start
negative.
and the finish-milling circle
J > {(Data parameter P269
setting value * cutter radius) +
cutter radius}*2.
Cutter radius under the helix <
Width of G33/G34 rectangle groove
along with the Y axis direction
{( J/2) – cutter radius}
0<J≤99999.999mm,
it
is
the
absolute value when in the
negative
Width of G35/G36, G37/G38 rectangle
groove along with the Y axis direction
The vectior of the circular arc center
K
-99999999～99999999（mm）
relative start along with the Z axis
(Arc/helix interpolation and scaling)
1～99999
Fixed cycle repeated times
1～99999
Repeated calling times of subprogram
The cutting width increment of the
Cutter diameter>L>0
G22/G23 inner circle groove cycle inside
the XY plane
L
Cutter diameter>L>0, it is the
absolute value when in the
negative.
M
O
16
in the specified plane
Cutter radius ≤ L ≤99999999mm,
The distance between the G37/G38
it is the absolute value when in
finish-milling start and rectangle edge X
the negative.
axis direction.
The setting of data parameter
P204
0～99999
N
The cutting width increment of G33/G34
0～999
0～99999
Miscellanous function output, program
execution schedule, subprogram call
Sequence number
Parameter
sequency
on-line modification)
Program name
number
(G10
Chapter Three
Add.
Component Program Configuration
Resolution range
0～99999.9999（ms）
1～99999
Dwell time
Subprogram number call
-9999.9999～9999.9999
P
Function meaning
Scaling
The dwell time at the bottom of the hole
Data parameters P281~282
in the canned cycle or the time at the
point R when retracting.
Q
-99999999～99999999（mm）
-99999.999～99999.999（mm）
The setting of data parameter
P205
S
00～04
T
the bottom of the hole in canned cycle
Circular
arc
radius/angle
offset
value/corner value
The R plane in the canned cycle
Spindle rotation specification
Multi-gear spindle output
The setting of data parameter
P206
The setting of data parameter
P175~179
U
The cutting detpth or the offset value at
VOLUME I
PROGRAMMING
R
-99999.999～99999.999（mm）
Tool function
Axle name address
The resolution range of the U is
I/2≥|U|≥D/2, the smaller value in
Corner arc radius in canned cycle
J/2
The setting of data parameter
P175~179
V
The distance from the unprocess plane
V>0
when cutting at the rapid traverse rate
The setting of data parameter
P175~179
W
W>0 (It should be exceeded the
slot-bottom position at the first,
and
then
directly
machining
based upon its bottom
The setting of data parameter
P175~179
X
Axle name address
-99999.999～99999.999（mm）
0～9999.999（S）
Axle name address
The first cutting distance of Z axis
direction from R plane in the canned
cycle
Axle name address
Coordinate
address
along
with
X
direction
Dwell time specification
17
GSK218MC Series Machining CNC System
Add.
Resolution range
Function meaning
The setting of data parameter
Y
P175~179
-99999.999～99999.999（mm）
The setting of data parameter
Z
Programming & Operation Manual
P175~179
-99999.999～99999.999（mm）
Axle name address
Coordinate
address
along
with
Y
along
with
Z
direction
Axle name address
Coordinate
address
direction
It is the overall restriction values of CNC equipment in table 3-1-3-1, regardless of the one of the
VOLUME I
PROGRAMMING
machine tool. And therefore, it is important to program based upon the comprehension of the
programming limit for referring this manual and the one of the machine tool manufacturer.
Note: The length of each code word should be less than 79 characters.
3.2
General Structure of Program
Program divides into Main program and subprogram. Usually, the CNC moves based upon the
indication of the main program; if the code for calling the subprogram on the main program, the CNC
is then operated according to subprogram; when meeting the main program code return on
subprogram, CNC is then returned to the next program for that the main program calls the
subprogram block to be consecutively performed. The program motion sequence is as Fig. 3-21.
Main program
Subprogram
Command 1
Command 1
Command 2
Command 2
……
……
Subprogram
command call
Command N
……
……
M30
……
M99 main
program return
Fig. 3-2-1
The composition structure of main program and subprogram are consistent.
When some one fixed sequence exists and occurs repeatedly in the program, which can be
regarded as subprogram, and then save to the register in advance instead of writing again to simplify
the program. Subprogram can be called in the Auto mode, generally, the calling can be performed by
18
Chapter Three
Component Program Configuration
M98 among main programs, and also, the called subprogram can be called other subprograms. The
called subprogram from the main program is called as the First Subprogram, and there are four
subprograms can be called (Refero to the Fig. 3-2-2). The last block of the subprogram can be
returned to the main program by M99 code, call the next block of the subprogram to be consecutively
performed. (If the last block of the subprogram is ended using the M02 or M03 code; the function is
same as the M99, return to the main program, and then call the next block of the subprogram to be
consecutively performed.)
When the end of the main program is M99, the program is repeatedly performed.
Main
program
Subprogram
O10000;
…
…
…
M98 P20000;
…
…
…
…
M99;
O20000;
…
…
…
M98 P30000;
…
…
…
…
M99;
O30000;
…
…
…
M98 P40000;
…
…
…
…
M99;
First nesting
Second nesting
Third nesting
Fig. 3-2-2
Subprogram
Subprogram
O40000;
…
…
…
VOLUME I
PROGRAMMING
O00001;
…
…
…
M98 P10000;
…
…
…
…
M30;
Subprogram
…
…
…
…
M99;
Quadruple
nesting
Quadruple subprogram nesting
One subprogram calling code can be consecutively and repeatedly called the same subprogram,
and up to 9999 times can be repeatedly called.
3.2.1
Subprogram Compiling
Compile a subprogram based upon the following format:
; Subprogram No.
O
……
……
Subprogram
……
M99;
Subprogram end
Fig. 3-2-1-1
Write the subprogram No. following the address O at the beginning of the subprogram, the
subprogram, at last, is M99 code (M99 compiling formate is as the above-mentioned figure).
19
GSK218MC Series Machining CNC System
3.2.2
Programming & Operation Manual
Subprogram Calling
The subprogram is performed by main program or calling the code. The subprogram calling code
formate is as follows:
L
M98 P
Repeat the calling times
The called subprogram
series No.
Fig. 3-2-2-1
● If the repeated times are omitted, the repeated times will be regarded as 1.
(Example) M98 P1002L5 ;
(The subprogram No.1002 is consecutively called for 5 times)
VOLUME I
PROGRAMMING
● The performance sequence calling from main program to subprogram.
1 2 3
Main program
Subprogram
N0010 …… ;
O10100 ;
N0020 …… ;
N1020…… ;
N0030 M98 P10100L3 ;
N1030…… ;
N0040 …… ;
N1040…… ;
N0050 M98 P10100 ;
N1050…… ;
N0060…… ;
N1060 …… M99 ;
Fig. 3-2-2-2
Calling the subprogram in the subprogram is same as the calling in the main program.
Note 1: When the specified subprogram number by address P can not be indexed; the alarm occurs.
Note 2: The subprogram from No. 90000 to 99999 are the system reserved. The system can be performed the content
of the subprogram instead of display the content when user calls these subprograms.
Note 3: Up to 4 layers can be nested for the subprogram calling.
3.2.3
Program End
Program begins from its name which is ended by M02, M30 or M99 (Refer to the Fig. 3-2-2-2). If
the program end code is detected in the execution of the program: M02, M30 or M99; The program is
performed and then becomes to restting state when M02, M30 code ends; Whether the bit 4 of
parameter No.33 for controlling the M30 returns to the beginning of the program; Whether the bit 2 of
parameter No.33 for controlling the M02 returns to the beginning of the program. If M99 code ends,
return to the beginning of the program, and then the program is circularly performed; If the M99, M02
and M30 are ended in the subprogram, return to the program of the subprogram calling, and then
perform the following blocks continuously.
20
Chapter Four
CHAPTER FOUR
4.1
Preparatory Function G Code
PREPARATORY FUNCTION G CODE
Type of Preparatory Function G Code
The preparatory function is expressed by G code and its following numbers, which specifies the
meaning of its block. G codes are divided into the following two types.
Table 4-1-1
Type
Meaning
The G code is enabled only in the block in which it
One-shot code
VOLUME I
PROGRAMMING
is specified
It is always effective before the other G codes in
Modal G code
the same group.
(Example) G01 and G00 are the modal G code in the same group.
G01 X ＿ ;
Z ＿＿＿ ; G01 enabled
X ＿＿＿ ; G01 enabled
G00 Z＿＿ ; G00 enabled
The system bit 7 of parameter No. 0 is common machining mode when it is set to 0. It is the
high-velocity high-accuracy machining mode when the bit 7 of No. 0 sets to 1.
Note 1: F: It is indentical with the common machining mode
T: high-velocity high-accuracy machining mode
Note 2: Refer to the system parameter table for details.
Table 4-1-2
code
*G00
Group
Code form
G00 X_Y_Z_
01
G01 X_Y_Z_F_
G01
G02
G02
X_Y_
R_
F_；
High-velocity/
high-accuracy mode
enabled or not
G
G code and its function
T
T
T
Function
Positioning (Rapid
traverse)
Linear interpolation
(Cutting feed)
Circular arc interpolation
CW (Clockwise)
21
GSK218MC Series Machining CNC System
code
Group
Code form
G03
G03
G04
G10
00
G10 L_N_P_R_
G11
VOLUME I
PROGRAMMING
16
G13
G16
G16
*G17
02
G19
G20
G21
06
09
G25
G28
22
interpolation and cutter compensation
Specify this command in a single block
G24 X_Y_Z_R_I_J_D_F_K_
G25 X_Y_Z_R_I_J_D_F_K_
G26 X_Y_Z_R_I_J_D_F_K_
G26
G27
Write in the block, it is used in the both arc
G23 X_Y_Z_R_I_L_W_Q_V_D_F_K
G23
G24
F
G22 X_Y_Z_R_I_L_W_Q_V_D_F_ K
G22
00
G27
G28
Programmable data input
F
11
X_Y_Z_
CCW (Counter Clockwise)
F
F
G15
Circular arc interpolation
Dwell, Exact stop
F
G13
Function
F
F
G12 X_Y_Z_ I_J_K_
*G12
G18
T
G04 P_ or G04 X_
*G11
*G15
I_J_
High-velocity/
high-accuracy mode
enabled or not
G
Programming & Operation Manual
Programmable data input
mode cancel
Stored stroke check
function ON
Stored stroke check
function OFF
Polar coordinate code
cancel
Polar coordinate code
XY plane selection
F
ZX plane selection
YZ plane selection
F
F
F
F
F
F
T
T
Data input in inch
Data input in metric
Groove rough mill inner
circle CCW
Groove rough mill inner
circle CW
Finish mill circular inner
the whole-circle CCW
Finish mill circular inner
the whole-circle CW
Finish mill circular of
excircle CCW
Reference position return
check
Reference position return
Chapter Four
code
Group
High-velocity/
high-accuracy mode
enabled or not
G
Preparatory Function G Code
Code form
G29
G29
T
G30Pn
G30
G31
T
G31
F
G33
F
G33X_Y_Z_R_I_J_L_W_Q_V_U_D_F_K
G34X_Y_Z_R_I_J_L_W_Q_V_U_D_F_K
G34
F
F
G35 X_Y_Z_R_I_J_L_ U_D_F_K_
G35
09
Return from the reference
position
2nd, 3rd and the 4th
reference position return
Skip function
Finish mill circular of
excircle CW
Rectangle groove rough
mill CCW
Rectangle groove rough
mill CW
Finish mill circular inner
F
the rectangular groove
CCW
G36 X_Y_Z_R_I_J_L_ U_D_F_K_
G36
G37 X_Y_Z_R_I_J_L_ U_D_F_K_
G37
G38 X_Y_Z_R_I_J_L_ U_D_F_K_
G38
G39
G17
*G40
G41
07
G42
*G49
G40
G41
G18
G42
G19
G43
G44
G39
00
G44
G49
F
F
F
D_X_Y_
T
Finish mill circular inner
the rectangular groove CW
Finish mill circular out of
the rectangle CCW
Finish mill circular out of
the rectangle CW
Corner offset circular arc
interpolation
Cutter compensation
cancel
D_X_Z_
T
Left cutter compensation
D_Y_Z_
T
Right cutter compensation
G43
08
F
T
H_Z_
T
T
Tool length compensation
+ direction
Tool length compensation direction
Tool length compensation
cancel
23
VOLUME I
PROGRAMMING
G32 X_Y_Z_R_I_J_D_F_K_
G32
Function
GSK218MC Series Machining CNC System
code
*G50
G51
G53
Code form
High-velocity/
high-accuracy mode
enabled or not
G
Function
G50
T
Scaling cancel
G51 X_ Y_ Z_ P_
T
Scaling
Write in the program
T
Group
12
00
Programming & Operation Manual
VOLUME I
PROGRAMMING
system 1
Workpiece coordinate
G55
system 2
Workpiece coordinate
G56
05
Write in the block, it generally places at the
beginning of the program.
G57
T
system 5
Workpiece coordinate
system 6
00/01
G60 X_ Y_ Z_
T
Unidirectional positioning
G61
T
Exact stop mode
G62
T
Automatic corner override
G63
T
Tapping mode
G64
T
Cutting mode
G65 H_P# i Q# j R# k
T
Macro program code
G68 X_ Y_ R_
T
Coordinate rotation
G69
T
Coordinate rotation cancel
G61
14
*G64
G65
G68
*G69
G73
00
13
09
G73 X_Y_Z_R_Q_F_；
F
High-speed peck
machining cycle
G74
G74 X_Y_Z_R_P_F_；
F
Counter tapping cycle
G76
G76 X_Y_Z_Q_R_P_F_K_；
F
Fine boring cycle
F
Canned cycle cancel
*G80
24
Workpiece coordinate
Workpiece coordinate
G59
G63
system 3
system 4
G58
G62
system selection
Workpiece coordinate
G54
G60
Machine tool coordinate
Write along with other programs in the
block
Chapter Four
code
Group
Code form
G81 X_Y_Z_R_F_；
G81
G82 X_Y_Z_R_P_F_；
G82
High-velocity/
high-accuracy mode
enabled or not
G
Preparatory Function G Code
F
F
Function
Drilling cycle (spot drilling
cycle)
Drilling cycle, counter
boring cycle
G83 X_Y_Z_R_Q_F_；
F
Peck drilling cycle
G84
G84 X_Y_Z_R_P_F_；
F
Right tapping cycle
G85
G85 X_Y_Z_R_F_；
F
Boring cycle
G86
G86 X_Y_Z_R_F_；
F
Boring cycle
G87
G87 X_Y_Z_R_Q_P_F_；
F
Back boring cycle
G88
G88 X_Y_Z_R_P_F_；
F
Boring cycle
G89
G89 X_Y_Z_R_P_F_；
F
Boring cycle
*G90
G91
G92
*G94
G95
03
00
04
Write in the block
G92 X_Y_Z_
15
T
Absolute command
Increment command
Floating coordinate
system setting
G94
T
Feed per minute
G95
T
Feed per rotation
G96S_
G96
T
T
G97S_
*G97
VOLUME I
PROGRAMMING
G83
Constant cycle-speed
control (Cutting speed)
Constant cycle-speed
T
control cancel (Cutting
speed)
Return to the initial plane
*G98
10
Write in the block
G99
T
in canned cycle
Return to the R point plane
in canned cycle
Note 1: If the modal code is shared with a same block with the one-shot modal, and the one-shot modal shoud be
considered in priority; simultaneously, change the corresponding mode based upon the other modal codes in
a same block, instead of executing them.
Note 2: The system is on G code state of which this G code is with * when the power is turned on. (Partial G codes are
25
GSK218MC Series Machining CNC System
Programming & Operation Manual
determined by bits 0~7 of parameter No.:31)
Note 3: The G codes of the 00 goup are the non-modal G codes other than the G10, G12 and G92.
Note 4: If th G codes without showing in the G code table are used, the alarm then occurs; perhaps, the alarm will also
be generated if the G code without the optional function is specified.
Note 5: Several different G codes can be specified in a same block. In principle, two or more G codes in a same group
can not be specified in a same block. If a same code that does not alarm in a same block is set, it is subject to
the following G codes.
Note 6: The G codes of 01 and 09 groups are shared with a same block. In the canned cycle modal, if the G code in
group 01 is specified, the canned cycle will be automatically cancelled and then turn into G80 state.
Note 7: G codes are separately expressed by each group based upon the different types. Whether clear the G codes
of each group when resetting or in the ESP, which are set by both the bits 0~7 of parameter No.35 and bits
0~7 of parameter No.36.
Note 8: When the rotation scaling codes and the codes in the 01 or 09 group are shared with a same block, it is better
VOLUME I
PROGRAMMING
to subject to the rotation scaling code; simultaneously, change the modal of 01 or 09 group. The system will
alarm when the rotation scaling code and the code in 00 group are shared with a same block.
4.2
Simple G Code
4.2.1
Rapid Positioning G00
Format: G00 X_Y_Z_
Function: The G00 code moves a tool to the position in the workpiece coordinate system specified
with an absolute or an increment code at a rapid traverse rate.
Either of the following tool paths can be selected according to bit 1 of parameter No.12.
(Refer to the Fig. 4-2-1-1)
1. Linear interpolation positioning: The tool path is identical with linear interpolation (G01).
The tool is positioned within the shortest possible time at a speed that is not more than the
rapid traverse rate for each axis.
2. Nonlinear interpolation positioning: The tool is separately positioned at the rapid traverse
rate for each axis. The tool path, generally, is not a straight line.
Non-linear
interpolation position
End
Start
Linear interpolation
position
End
Fig. 4-2-1-1
26
Start
Chapter Four
Preparatory Function G Code
Explanations:
1. After executing the G00, the modal of current tool movement method turns into G00 by
system. Whether the system default mode when the power is turned on is G00 (The
parameter value is 0) or G01 (The parameter value is 1) by changing the value of bit 0 of
parameter No.31.
2. Fail to move the positioning parameter tool without specification. The system is only
changed the modal (G00) of the current tool movement mode
3. Both G00 and G0 are the equivalent format.
4. The X, Y, Z and the 4th axis and G0 speed are determined by parameter P88~P91.
Restriction:
cutting feedrate of the following machining section.
For example:
G0 X0 Y10 F800;
G1 X20 Y50;
Rapid feed using the speed set by system parameter
Use the feedrate of F800
Rapid positioning speed is adjusted by buttons on the operation panel (Refer to the Fig. 4-2-1-2),
F0, 25%, 50% and 100%; F0 speed is set by data parameter P93; general-purpose for each axis.
218MC, 218MC-H, 218MC-V buttons
Fig. 4-2-1-2
218MC-U1 button
The button of rapid feedrate
Note: It is important to note the worktable and workpiece positions when programming to prevent the tool from
impacting.
4.2.2
Format:
Linear Interpolation G01
G01 X_ Y_ Z_ F_
Function: The tool along a line moves to the specified position based upon the feedrate (mm/min.)
from parameter F.
27
VOLUME I
PROGRAMMING
Rapid traverse rate is determined by parameter, for example, set F speed in G0 code, it is the
GSK218MC Series Machining CNC System
Programming & Operation Manual
Explanations:
1. X_ Y_ Z_ is the end coordinate value. It is concerned to the concept of coordinate system,
refer to the Sections 2.4.1～2.4.4.
2. The feedrate specified in F is always enabled unitl a new value is specified. The feedrate
specified with F code is calculated along with the linear path interpolation. If the F code
does not specify in program, the feedrate uses the system ON default F value. (Refer to
the data parameter P87 for the setting).
Program example (Refer to the Fig. 4-2-2-1)
Y axis
G01 X200 Y100 F200 ；
End
VOLUME I
PROGRAMMING
100
Note: The speed of each axis direction:
G01 Xα Yβ ZγFf ；
Start
200
X axis
In this block
Feedrate of X axis direction:
Feedrate of X axis direction:
Feedrate of X axis direction:
L=
Fig. 4-2-2-1
Notice:
1. The code parameters other than the F are the positioning parameter. Set the upper-limit value of
the feedrate F by the data parameter P96. If the actual cutting feed (The feedrate after using the
override) exceeds the upper-limit, which is then restricted at the upper-limit. Its unit is mm/min. If the
actual cutting feedrate (The feedrate after using the override) is lower than the lower-limit, which is
then retricted on the lower-limit, and its unit is mm/min.
2. The tool does not move when the G01 is not specified the positioning parameter. The system is
only changed the modal of current tool movement which is the G01. Wheter the system default mode
is G00 (When the parameter value is 0) or G01 (When the parameter value is 1) can be set when the
power is turned on by changing the value of the bit 0 of the parameter No.:31
4.2.3
Circular Arc (Helical) interpolation G02/G03
A. Circular arc interpolation G02/G03
28
Chapter Four
Preparatory Function G Code
Both G02 and G03 are specified as follows:
The circular arc interpolation inside the plane is that its path is performed along with the specified
rotation and radius (or center) in the specified plane. Thanks to the recognized start and end can not
fully affirmed the arc path, and therefore, it is necessary to offer:
¾
Arc roataion direction (G02, G03)
¾
The plane of arc interpolation (G17, G18, G19)
¾
Center coordinate or radius is led out two code formats, center coordinate I, J and K or
radius R programming.
The interpolation calculation can be performed in the coordinate system only when the
above-mentioned 3 cases are fully affirmed.
The arc interpolation can be performed by following code; and the tool can be operated along with
VOLUME I
PROGRAMMING
the arc, refer to the following figure:
Arc in the XY plane
G17
G02
X_Y_
G03
R_
F_；
I_J_
Arc in the ZX plane
G18
G02
G03
X_Z_
R_
F_；
I_K_
Arc in the YZ plane
G19
G02
G03
Y_Z_
R_
F_；
J_K_
Table 4-2-3-1
Item
Specified content
Command
G17
1
Plane specification
G18
G19
2
Revolving direction
G90 method
3
End position
G91 method
Description
Specification of arc on XY
plane
Specification of arc on ZX
plane
Specification of arc on YZ
plane
G02
CW
G03
CCW
Two axes of X, Y or
End position coordinate in
Z
workpiece coordinate system
Two axes of X, Y or
The coordinate for the end
Z
relative to the start
29
GSK218MC Series Machining CNC System
The vector from start to
4
Two axes of I, J or K
center
Programming & Operation Manual
The position coordinate for
the center relative to the start
Arc radius
R
Arc radius
Feedrate
F
Tangent velocity of arc
5
It is so called the CW and CCW, which is viewed from + to - direction of Z axis (Y axis, X axis) for
the XY plane (ZX plane, YZ plane) in the right-hand rectangular coordinate system; refer to the Fig.
4-2-3-1.
X
Y
Z
G03
G03
G03
G02
VOLUME I
PROGRAMMING
G02
G02
Z
X
Y
G18
G17
G19
Fig. 4-2-3-1
Setting the bit 1 and 2 of parameter No. 31 can be specified the defaulted plane modal
information when starting up.
Specify the arc end by parameter word X, Y or Z. The corresponding G90 command is indicated
by absolute value, the G91 by increment value, and the increment value is the coordinate for the end
relative to the start. The arc center is specified by parameter word I, J or K, which are separately
corresponding to the X, Y or Z. I, J or K parameter value, are the coordinate (Simply, it is temporary to
regard the start as the coordinate origin, the coordinate of the center located) for the center relative to
the arc start, whenever in the absolute mode G90 or in the relative mode G91, which are the
increment value included with the symbol. Refer to the Fig. 4-2-3-2.
End（X,Y)
Start
Start
J
Center
I
30
End（Y,Z)
End（Z,X)
Start
K
I
Center
K
Center
J
Chapter Four
Preparatory Function G Code
I, J or K is with the symbol based upon the center relative to the start direction. Arc center also
can be specified by radius R other than the I, J or K.
G02 X_ Y_ R_ ；
G03 X_ Y_ R_ ；
1. In this case, the following two arcs can can be drawn, one is the circle more than 180°, the
other is the one less than 180°. The arc radius more than 180° is specified by negative value.
(Example: Fig. 4-2-3-3)
When the arc of ① is less than 180°.
G91 G02 X60 Y20 R50 F300 ；
When the arc of ② is more than 180°.
G91 G02 X60 Y20 R-50 F300 ；
R=50
End
1
2
Start
R=50
Fig. 4-2-3-3
2. If the arc that equals to 180° can be programmed by both the I, J or K and the R:
Example: G90 G0 X0 Y0；G2 X20 I10 F100；
Equal to G90 G0 X0 Y0；G2 X20 R10 F100
or
G90 G0 X0 Y0；G2 X20 R-10 F100
Notice: The + or – value of the180° arc R is regardless of the motion path of the arc.
31
VOLUME I
PROGRAMMING
Fig. 4-2-3-2
GSK218MC Series Machining CNC System
Programming & Operation Manual
3. If the arc that equals to the 360° is only can be programmed by I, J or K.
(Program example):
Y
100
R50
End
60
Start
R60
40
90
120 140
200
X
VOLUME I
PROGRAMMING
Fig. 4-2-3-4
The tool path programming of the Fig. 4-2-3-4 is as follows:
1. In absolute programming
G90 G0 X200 Y40 Z0；
G3 X140 Y100 R60 F300；
G2 X120 Y60 R50；
Or
G0 X200 Y40 Z0；
G90 G3 X140 Y100 I-60 F300；
G2 X120 Y60 I-50；
2. In incremental programming
G0 G90 X200 Y40 Z0；
G91 G3 X-60 Y60 R60 F3000；
G2 X-20 Y-40 R50；
Or
G0 G90 X200 Y40 Z0；
G91 G3 X-60 Y60 I-60 F300；
G2 X-20 Y-40 I-50；
Restrictions:
1. When the address I, J or K and R are simultaneously specified by program, the arc specified by
R is prior, and the others are omitted.
2. If the arc radius parameter does not specify from the start to the arc center, the system will then
alarm.
3. If you want to interpolate a whoel circle, only the parameter I, J or K can be specified from the
start to arc center, instead of specifying the R.
32
Chapter Four
Preparatory Function G Code
4. It is note the setting of the coordinate plane when the arc interpolation is performed.
5. Tool is invariables if X, Y and Z are omitted, that is the start and end are shared with a same
position, and the R is specified (For example: G02R50;).
B. Helical interpolation
Code format: G02/G03
Circular arc on XY plane
G02
G17
I J
Xp Yp Zp
F
G03
R
G02
G18
VOLUME I
PROGRAMMING
Circular arc on ZX plane
I K
Xp Yp Zp
F
G03
R
Circular arc on YZ plane
G02
G19
J K
Xp Yp Zp
F
G03
R
Fig. 4-2-3-5
Function: The tool from the current point moves to the specified position with the helical path based
upon the feedrate appointed by parameter F.
Explanation:
Z
Tool path
Y
X
The feedrate along with the 2-arc
interpolation axis circle is the specified one.
Fig. 4-2-3-6
The previous two-digit of code parameters are positioning parameter. The parameter words are
the 2 axes numbers (X, Y or Z) inside the current plane. These two positioning parameter are
specified a tool that should be moved to the position inside the current plane. The parameter words of
the 3rd code parameter is the linear axis other than the arc interpolation axis. Its parameter value is
the helical height. The meanings and restrictions of other code parameters are identical with the
33
GSK218MC Series Machining CNC System
Programming & Operation Manual
circular arc interpolation.
If the system can not machined a circle based upon the offered code parameter, the system is
then returned the incorrect information. The modal of the current tool movement method changes to
G02/G03 by system after it executes.
The feedrate along with two arc interpolation axes circle is specified. The command method is to
simply add a move axis which is not a circular arc interpolation axis. An F code specifies a feedrate
along a circular arc. Therefore, the feedrate of the linear axis is as follows:
F C =F *
Length of linear axis
Length of circular arc
VOLUME I
PROGRAMMING
Affirm that the feedrate of linear axis is less than any of the restriction values.
Restriction:
It is note the coordinate plane selection when the helical interpolation is performed.
4.2.4
Absolute/Incremental Programming G90/G91
Format: G90/G91
Function: The code axis movement value method are included the absolute value code and the
incremental value code.
The absolute value code is programmed with the coordinate value by the end of axis movement,
and the end position is concerned with the concept of the coordinate system; refer to the Sections
2.4.1～2.4.4.
The incremental value code is directly programmed by the relative movement value of the axis.
The incremental value is regardless of its coordinate system, it only needs to be offered the
movement direction and distance that of the end position relative to the start one.
The absolute value code and the increment one are separately used by G90 and G91.
Y
70
End
Start
30
X
40
100
Fig. 4-2-4-1
34
Chapter Four
Preparatory Function G Code
The movement from start to end in the Fig. 4-2-4-1 is programmed by absolute G90 and
increment G91 are shown below:
G90 G0 X40 Y70；
or G91 G0 X－60 Y40 ；
The above-mentioned methods can be performed the same operation. User can use it flexibly
based upon the requirements.
Explanations:
¾
Parameter without code can be written to the block along with other codes.
¾
G90 and G91 that are the modal values are shared with a same group, that is, the G90
mode is specified.
System parameter:
Setting the bit 4 of parameter No.31 can be specified whether the default positioning parameter
is G90 (When the parameter is 0) or G91 (When the parameter is 1) mode when starting up.
4.2.5
Dwell (G04)
Format: G04 X_ or P_
X, P: Specify a time
Function: G04 executes a dwell, delay performs based upon the specified time and then execute the
next block. In addition, in the cutting method, the exact stop detection is performed in the
G64, which can be specified the dwell. The feed method G95 per rotation specifies the
dwell by the bit 0 of parameter No. 34.
Table 4-2-5-1 Command value range of dwell time (Command by X)
The least movement unit
Command value range
No.5#1=0
0.001～9999.999
No.5#1=1
0.0001~9999.999
Dwell time unit
s or rev
Table 4-2-5-2 Command value range of dwell time (Command by P)
The least movement unit
Command value range
Dwell time unit
No.5#1=0
1~99999.999
0.001s or rev
No.5#1=1
1~99999.999
0.0001s or rev
35
VOLUME I
PROGRAMMING
mode is the default before the G91 does not specify; and the G91 is enabled unitl the G90
GSK218MC Series Machining CNC System
Programming & Operation Manual
Explanations:
1. G04 is the one-short modal code, which is only enabled at the current line.
2. X value is enabled when the X and P parameters are displayed together.
3. When the X and P values are set as negative, the alarm may occur.
4. The system does not perform the dwell when X and P are not specified.
5. The alarm may be generated if the axes commands (Y, Z, U, V, W, A, B or C) other the X are
specified after the G04.
4.2.6
Single Direction Positioning (G60)
VOLUME I
PROGRAMMING
Format: G60 X_ Y_ Z_
Overrun
value
Dwell
Start
Start
End
Dwell
Fig. 4-2-6-1
Function: When the accuracy positioning should be performed for eliminating the machine backlash,
which can be performed the accuracy positioning from one direction by using G60.
Explanations:
G60, which is a one-shot G code (Set whether it is modal value by the bit 0 of parameter No.
48), can be enabled only in the specified block.
Parameter X, Y and Z are indicated as the end coordinate values in the absolute programming
and the tool movement distance in the increment programming. In the tool offset, the path of
unidirectional positioning is the one after the tool compensation when the unidirectional positioning is
performed.
The marked overrun in the above-mentioned figure can be set by the system parameters P335,
P336, P337 and P338, and the dwell time can be set by the P334, as well the positioning direction
can be determined by setting the +/- of the overrun. Refer to the system parameter for details.
For example:
G90 G00 X-10 Y10；
G60 X20 Y25；
36
(1)
Chapter Four
Preparatory Function G Code
If the system parameter are P334 = 1, P335 = -8 and P336 = 5, tool path is AB→ dwell 1s→BC
for the (1) statement.
Y
C(20,25)
B(28,20)
20
Dwell for 1S
A(-10,10)
10
VOLUME I
PROGRAMMING
X
—10
0
10
20
30
Fig. 4-2-6-2
System parameter:
Table 4-2-6-1
P334
Dwell time for the single direction positioning (Unit: s)
P335
Single direction positioning and overshoot along with the X axis (Unit: mm)
P336
Single direction positioning and overshoot along with the Y axis (Unit: mm)
P337
Single direction positioning and overshoot along with the Z axis (Unit: mm)
P338
Single direction positioning and overshoot along with the 4th axis (Unit: mm)
Note 1: The symbols of the data parameter P335～P338 are expressed the unidirectional positioning,
and the value of the parameters are indicated as the overrun
Note 2: overrun value >0, the positioning direction is +.
Note 3: overrun value <0, the positioning direction is -.
Note 4: overrun value =0, do not perform the unidirectional positioning.
4.2.7
System Parameter On-Line Update
Function: This function is used for setting or modifying the values of the cutter radius, length offset,
external zero offset value, workpiece zero offset value, additional workpiece zero offset,
data parameter and bit parameter in the program.
37
GSK218MC Series Machining CNC System
Programming & Operation Manual
Format:
G10 L50 N_P _R_；
Set or modify the bit parameter
G10 L51 N_ R_；
Set or modify the bit parameter
G11；
Cancel the parameter input method
Parameter definition:
N: Parameter Number. The parameter series No. to be modified.
P: Parameter bit number. The parameter bit No.
R: Modification value. It is used for specifying the value after the parameter is modified.
The modification specification value can be performed based upon the following codes; refer to
the relative Chapters for details:
VOLUME I
PROGRAMMING
G10 L2 P_X_Y_Z_A_B_;
Set and alter the external zero offset value or the workpiece zero
offset value
G10 L10 P_R_;
Set or alter the length offset value
G10 L11 P_R_；
Set or alter the length wore value
G10 L12 P_R_；
Set or alter the radius offset value
G10 L13 P_R_；
Set or alter the radius wore value
G10 L20 P_ X_Y_Z_A_B_；
Set or alter the additional workpiece zero offset value
Note 1: In the parameter input method, do not specify other NC statements other than the note one.
Note 2: The G10 should be separately specified in block; otherwise, the alarm may occur; It is necessary to
cancel the parameter input method by G11 after using the G10 so as not to affect the normal use for the
program.
Note 3: The parameter value altered by G10 should be met the range of the system parameter, if does not, the
alarm will issue.
Note 4: It is essential to cancel the modal code of the canned cycle before operating the G10; otherwise the
system may alarm.
Note 5: The parameter should be restarted after the power is turned off that can not be modified by G10.
Note 6: G20, G21 can not be used the on-line alteration by G10.
Note 7: G10 on-line alters the external zero offset value, workpiece zero offset value, additional workpiece zero
offset value and tool offset value; when it is modified in the G91 modal, the commanded offset and the
current one will be overlapped by system; in the G90 modal, it is modified based upon the specified offset
value.
Note 8: Cancle G10 modal when performing the M00, M01, M02, M30, M99, M98 and 06.
Note 9: The bit 7 of parameter No. 0 (Selection mode 0: Common mode, 1: High-velocity and high-accuracy mode)
does not support the G10 on-line modification.
4.2.8
Workpiece Coordinate System G54～G59
Function: Specify the current workpiece coordinate system. Select a workpiece coordinate system
by specifying a worpiece coordinate system G code in a program.
38
Chapter Four
Preparatory Function G Code
Format: G54～G59
Explanations:
1. Without code parameters
2. The system, itself, can be set 6 workpiece coordinate systems, which any of the coordinate
can be selected by codes G54~G59.
G54 ---------------- Workpiece coordinate system 1
G55 ---------------- Workpiece coordinate system 2
G56 ---------------- Workpiece coordinate system 3
G57 ---------------- Workpiece coordinate system 4
G58 ---------------- Workpiece coordinate system 5
3. The system displays the performed workpiece coordinate system G54～G59, G92 or the
additional workpiece coordinate system before the power OFF.
4. When different workpiece coordinate systems are called in a block, specify a movement axis,
and then position to the coordinate point under a new workpiece coordinate system; the
coordinate will turn into its corresponding coordinate value under a new workpiece coordinate
system without specifying a movement axis, however the actual machine’s position is invariable.
Example: The coordinate system origin of G54 corresponding with its machine coordinate is (10,
10, 10)
The coordinate system origin of G55 corresponding with its machine coordinate is (30, 30,
30)
The absolute coordinate of the end and the machine coordinate are shown below when
performing the program based upon its sequence:
Table 4-2-8-1
Program
Absolute coordinate
Machine coordinate
50, 50, 50
60, 60, 60
G55 X100 Y100
100, 100, 30
130, 130, 60
X120 Z80
120, 100, 80
150, 130, 110
G0 G54 X50 Y50 Z50
5. G10 is available to change an external workpiece zero offset value or workpiece zero offset
value. Refer to the following methods:
With the code G10 L2 Pp X_Y_Z_
P=0:
External workpiece zero offset value (Basis offset value).
P=1 to 6:
The workpiece zero offset from workpiece coordinate systems 1 to 6.
X_Y_Z_:
For an absolute value code (G90), workpiece zero offset value of each axis.
For an incremental value code (G91), value to be added (The result of
addition becomes the new workpiece zero offset) to the set workpiece zero
offset for each axis.
39
VOLUME I
PROGRAMMING
G59 ---------------- Workpiece coordinate system 6
GSK218MC Series Machining CNC System
Programming & Operation Manual
With the G10 command, each workpiece coordinate system can be changed separately.
Workpiece
coordinate
system 1
（G54）
Workpiece
coordinate
system 3
（G56）
Workpiece
coordinate
system 2
（G55）
Workpiece
coordinate
system 4
（G57）
Workpiece
coordinate
system 5
（G58）
Workpiece
coordinate
system offset
Mechani
cal zero
Workpiece
coordinate
system 6
（G59）
VOLUME I
PROGRAMMING
Machine tool
reference position
Fig. 4-2-8-1
The above-mentioned Fig. 4-2-8-1 shows that the machine tool returns to the mechanical zero
manually after it is starting-up, which is established a machine tool coordinate system by mechanical
zero, and therefore, the machine tool reference position occrs and the workpiece coordinate system
confirms. The corresponding value of the workpiece coordinate system offset data parameter P10～
P13 is the integrated offset value for the 6 workpiece coordinate systems. And the 6 coordinate
systems are determined by the distance from the mechanical zero to the each coordinate system zer.
Z
Z
Y
Y
X
Workpiece
zero offset
Machine
tool zero
X
Fig. 4-2-8-2
Example: N10 G55 G90 G00 X100 Y20；
N20 G56 X80.5 Z25.5；
In the above-mentioned example, when the N10 block is executed, rapidly position to the
workpiece coordinate system G55 (X=100, Y=20). When the N20 block is executed, rapidly position
to the workpiece system G56, and the absolute value is automatically changed into coordinate value
(X=80.5, Z=25.5) under the G56.
40
Chapter Four
4.2.9
Preparatory Function G Code
Additional Workpiece Coordinate System
Also, there are 50 additional workpiece coordinate systems can be used other than the 6
workpiece coordinate systems (from G54 to G59).
Format: G54 Pn
Pn: Codes specifying the additional workpiece coordinate systems. The range of Pn:
1~50.
The setting and restriction of the additional workpiece coordinate system is consistent with the
workpiece coordinate system G54~G59.
G10 is available to set a workpiece zero offset value in an additional coordinate system. The
methods are shown below:
n=1 to 50 :
X_Y_Z_ :
Additional workpiece coordinate code.
Set the axis address and offset value offset by workpiece zero, the
specified value is a new offset one.
For an incremental value code (G91), specified value addes the current
offset value and gains a new offset value.
G10 command is available for separately changing each workpiece coordinate system.
4.2.10
Machine Coordinate System Selection G53
Format: G53 X_ Y_ Z_
Function: The tool is positioned to the cooresponding coordinate below its coordinte system at a
rapid traverse rate.
Explanations:
1. When the G53 is used within the program, its following code coordinate should be the
coordinate value below the machine tool coordinate system, and then the machine tool will
position to a specified place at a rapid traverse.
2. G53, is one-shot modal code, is only enabled at its current block regardless of the previous
defined coordinate system.
Restriction:
Select a machine coordinate system G53
When a command is specified the position on a machine coordinate system, the tool moves to
the position by rapid traverse. G53, which is used to select a machine coordinate system, is a
one-shot G code; that is, it is enabled only in the block in which it is specified on a machine
coordinate system. Specify an absolute command G90 for G53. When an incremental command G91
is specified, the G53 command is ignored. When the tool is to be moved to a machine-specified
position such as a tool change position, program the movement in a machine coordinate system
41
VOLUME I
PROGRAMMING
Code: G10 L20 Pn X_Y_Z_；
GSK218MC Series Machining CNC System
Programming & Operation Manual
based on G53.
Note: When G53 is specified, temperoarily cancel the current comensation and tool length offset, and then recover it
at the next compensation axis block to be buffered.
4.2.11
Floating Coordinate System G92
Format: G92 X_ Y_ Z_
Function: Set a floating workpiece coordinate system. Three code parameters are specified an
absolute coordinate value of the current tool in a new floating workpiece coordinate
system.
VOLUME I
PROGRAMMING
Explanations:
G92 floating
coordinate system
Mechanical
zero
achine coordinate
system origin
Fig. 4-2-11-1
1. The above-mentioned Fig. 4-2-11-1 shows that the cooresponding origin of the G92 floating
coordinate system is the value below the machine coordinate system, which is nothing to do with the
workpiece coordinate system.
1) Before calling a workpiece coordinate system
2) Before the machine tool zero return
Generally, the G92 floating coordinate system, is used for correcting the machining of the
temporary workpiece, is operated at the beginning of the program, or specify the G92 in MDI mode
before automatically operating the program.
2. There are two methods to confirm the floating coordinate system:
1) Coordinate system confirmation based upon a tool nose
42
Chapter Four
Preparatory Function G Code
Z
23
X
25
The Fig. 4-2-11-2 shows that, G92 X25 Z23, the tool nose position is treated as (X25, Z23) point
in the floating coordinate.
2) One fixed point at the tool handle is regarded as the reference point coordinate system:
Z
Reference
point
1200
600
X
Fig. 4-2-11-3
The Fig. 4-2-11-3 shows that the G92 X600 Z1200 is used; specify the coordinate system setting
(When one reference point on the tool handle is regarded as the start). And therefore, if it is
movement according to the absolute code in the program, and then the reference position moves to
the specified position; the tool length compensation should be added; its value is the difference from
the reference point to the tool nose.
Note 1: If the G92 setting coordinate system is used in the tool offset. The tool offset does not add for the tool length
compensation, and set the coordinate system by G92
Note 2: When, however, there is no alternative other than to cancel the cutter compensation before using the G92
code.
43
VOLUME I
PROGRAMMING
Fig. 4-2-11-2
GSK218MC Series Machining CNC System
4.2.12
Programming & Operation Manual
Plane Selection G17/G18/G19
Format: G17/G18/G19
Function: Select the planes for circular arc interpolation, cutter compensation or drilling, and boring.
In this case, the plane selection can be performed by G17/G18/G19.
Explanation: Without command parameter, the system is regarded as G17 by default when starting
up. Also, set the bit 1, 2 and 3 of the parameter No.: 31 to determine the default plane after
starting up. The corresponding relationships between codes and planes are as follows:
G17-------------XY Plane
G18-------------ZX Plane
G19-------------YZ Plane
VOLUME I
PROGRAMMING
The plane is invariable when the G17, G18 and G19 are not belonged to the specified block.
Example: G18 X_ Z_; ZX plane
G0 X_ Y_; Plane invariable (ZX plane)
Additional, the movement code is regardless of the plane selection. For example, the
following code shows that the Y axis is out of the ZX plane, and the Y axis movement is
regardless of the ZX plane.
G18Y_；
Prompt: At present, only the canned cycle in the G17 plane is supported. For the specification’s sake, it is better to
define the specified plane in the corresponding block when the programming is performed, specially when
several persons are shared with a same system. So that, the accident or abnormality may avoid due to the
incorrect programming.
4.2.13
Polar Coordinate Start/Cancel G16/G15
Format: G16/G15
Function:
G16 specifys the polar coordinate of positioning parameter, which means the beginning of the
method.
G15 specifys the polar coordinate of positioning parameter, which means the cancellation of the
method.
Explanation:
Without command parameter
Set the G16, the coordinate value can be inputted by polar coordinate radius and angle. The plus
direction of the angle is CCW of the selected plane first axis + direction, and the minus directionis CW.
Both the radius and angle can be specified in either absolute or incremental command (G90, G91).
After the G16 occurs, the 1st axis of the positioning parameter of the tool movement command
44
Chapter Four
Preparatory Function G Code
expresses the polar-radius below the polar coordinate system; the 2nd axis means the polar-angle
below the polar coordinate system.
Set the G15 to cancel the polar coordinate method, so that the coordinate value returns to use
the rectangle coordinate input.
The specification of the polar coordinate origin:
1. In the G90 absolute method, the workpiece coordinate system zero is regarded as the polar
coordinate origin when specifying by G16.
Command
position
Radius
Angle
When the angle is specified
by absolute value.
VOLUME I
PROGRAMMING
Actual
position
Angle
Command
position
Radius
Actual
position
When the angle is specified
by incremental value.
Fig. 4-2-13-1
2. In the G91 increment method, the current point is treated as the polar coordinate origin when
specifying by G16.
For example: Bolt hole circle (The zero of the workpiece coordinate system is set as the origin
of polar coordinate, select the X—Y plane).
--The zero of the workpiece coordinate
system is regarded as the origin of the
coordinate system.
-- Select the XY plane
Y
150°
270°
30°
100mm
X
Fig. 4-2-13-2
z
Specify an angle and a radius with absolute value
G17 G90 G16； Specifying the polar coordinate code and selecting the XY plane; setting the zero
point of the workpiece coordinate system as the origin of the polar coordinate
system
G81 X100 Y30 Z-20 R -5 F200；Specifying a distance of 100mm and an angle of 30°
Y150；
Specifying a distance of 100mm and an angle of 150°
45
GSK218MC Series Machining CNC System
z
Programming & Operation Manual
Y270；
Specifying a distance of 100mm and an angle of 270°
G15 G80；
Canceling the polar coordinate code
Specifying angles with incremental value and a polar-radius with absolute value
G17 G90 G16； Specifying the polar coordinate code and selecting XY plane; setting the zero of
the workpiece coordinate system as the origin of the polar coordinate system
G81 X100 Y30 Z-20 R -5 F200； Specifying a distance of 100mm and an angle of 30°
G91 Y120；
Specifying a distance of 100mm and an incremental angle of
+120°
Y120；
Specifying a distance of 100mm and an incremental angle of
+120°
VOLUME I
PROGRAMMING
G15 G80；
Canceling the polar coordinate code
In addition, when the polar coordinate is programmed, it is notice to set the current coordinate
plane. The polar coordinate plane is related with the current one; for example: G91, if the current
coordinate plane is G17, the X and Y axes components at the current tool position is the origin. If the
current coordinate plane is G18, and then the Z and X axes components at the current tool position is
the origin.
If the positioning parameter of the 1st hole circle command followed with G16 does not specify,
the current tool position of the system is regarded as the default position parameter of the hole circle.
At present, the 1st canned cycle code followed with the polar coordinate should be completed;
otherwise, the tool path will incorrect.
The parameter word of the tool movement command positioning parameter is related with the
concrete plane selection modal other than the hole circle followed with the G16. The default current
tool position, followed with the movement code, after using the G15 to cancel the coordinate, is the
start of the movement code.
4.2.14
Scaling Within Plane G51/G50
Format:
G51 X_ Y_ Z_ P_
(X.Y.Z: The absolute value code of scaling center coordinate value, P: Scling
each axis with same proportion)
…
The machining block of scaling
G50
Canceling the scaling
Or, G51 X_ Y_Z_ I_ J_ K_ (Each axis is separately performed acoording to different scaling (I, J
and K)
…
Machining block of scaling
G50
Canceling the scaling
Function:
46
Chapter Four
Preparatory Function G Code
The programmed shape is regarded as a center with the specified position by G51, scaling the
same or different proportion. It is necessary to point out that the G51 is specified (otherwise, the
unexpected situation may occur) with the single block and then cancel it by G50.
Y
P4
P3
P4́
P0
P3́
P1́
P2́
VOLUME I
PROGRAMMING
P1
P2
X
0
P0: Scaling center
'
Fig. 4-2-14-1 scaling (P1P2P3P4→ P1’P2’P3’P4 )
Expanations:
1. Scaling center: 3 positioning parameters X_Y_Z_ can be performed with G51, which are the
optional parameters. The positioning parameter is used to specify the scaling
center of the G51. If the positioning parameter does not specify, the system is set
the current position of the tool as the scaling center. The scaling center is always
specified with the absolute positioning mothod regardless of the current
positioning method is absolute or increment. Moreover, the parameter in G51 is
also indicated with the rectangular coordinate system in G51 code based upon
the polar coordinate G16 method.
Example: G17 G91 G54 G0 X10 Y10;
G51 X40 Y40 P2； Incremental method, scaling center is still the absolute
coordinate (40, 40) in the G54 coordinate system.
G1 Y90；
Parameter Y is still use the incremental method.
2. Scaling: The scaling is always expressed with the absolute method regardless of the current method is G90
or G91.
The scaling can be set in parameter other than specifying in program; data
parameter P330 sets the scaling multiplication of each axis; data parameter
P331~P333 are separately corresponding to scaling of the 1st, 2nd and 3rd axis; if
the scaling codes are not performed here, and when the bit 6 of parameter
No.:47 is set to 0, the scaling can be performed according to the setting value
from the data parameter P330; when the bit 6 of No.:47 is set to 1, the scaling is
then performed based upon the setting value of data parameter P331～P333.
If the parameter value of the parameters P or I, J and K are negative, the
47
GSK218MC Series Machining CNC System
Programming & Operation Manual
corresponding axes are performed the image.
3. Scaling setting: Whether the scaling function is used by the bit 5 of parameter No.: 60;
Whether the bit 3 of parameter No.: 47 sets the 1st axis is enabled; Whether the
bit 4 of parameter No.: 47 sets the 2nd axis is enabled; Whether the bit 5 of
parameter No.: 47 sets the 3rd axis is enabled; bit 6 of parameter No.: 47 set
the specification method of scaling override along with each axis (0: Using P
commands each axis; 1: Using I, J and K .
4. Cancel the scaling: After the scaling is cancelled by using the G50 code, and when the movement code is
followed, the coordinate scaling is cancelled; the tool position is the start point of the
movement code.
5. Scaling state can not specify the G codes (such as G27～G30) of reference position return
and the one (G53～G59, G54P1~G54P50, G92) of the coordinate system. If
VOLUME I
PROGRAMMING
these G codes must be specified, it should be specified after cancelling the
scaling function; otherwise, the system alarm occurs.
6. Tool does not draw out the ellipse path even if the arc interpolation and each axis are
specified the different scaling.
When the scaling along with each axis is different, and the arc interpolation is programmed by
radius R, its interpolation figure is as the Fig. 4-2-14-2 (The proportion of X axis is 2, Y is 1).
G90 G0 X0 Y100;
G51 X0 Y0 Z0 I2 J1;
G02 X100 Y0 R100 F500;
The above-mentioned commands are equal
to the following one:
G90 G0 X0 Y100;
G02 X200 Y0 R200 F500;
The proportion of radius R is scaled based
upon the bigger one of the I or J.
Y
the shape after scaling
（0，0） （100，0） （200，0）
Fig. 4-2-14-2
X
The scaling of circular arc interpolation
When the scaling along with each axis is different, and when the arc interpolation is programmed
by I, J and K, the arc is not performed and then the system alarms.
48
Chapter Four
Preparatory Function G Code
7. The scaling is disabled to the tool offset value, refer to the Fig. 4-2-14-3.
VOLUME I
PROGRAMMING
Fig. 4-2-14-3
The scaling of current compensation
Image program example:
Main program:
G00 G90；
M98 P9000；
G51 X50.0 Y50.0 I-1 J1；
M98 P9000；
G51 X50.0 Y50.0 I-1 J-1；
M98 P9000；
G51 X50.0 Y50.0 I1 J-1；
M98 P9000；
G50；
M30；
Subprogram:
O9000；
G00 G90 X60.0 Y60.0；
G01 X100.0 F100；
G01 Y100；
49
GSK218MC Series Machining CNC System
Programming & Operation Manual
G01 X60.0 Y60.0；
M99；
40 50 60
100
Y
VOLUME I
PROGRAMMING
0
40 50 60
100
X
Fig. 4-2-14-4
Restrictions:
1. In the canned cycle, the depth of Z axis cutting value, the 1st cutting depth distance W of
the return value d, Z and the movement scaling of the rapid cutting distance V, are all
disabled.
2. In the manual operation, the movement distance can not be increased or decreased by
scaling function.
Note 1: The position displays the coordinate value after scaling.
Note 2: There is an axis of the specification plane is performed the image, and its result is shown below:
1) Circular code……………Negative rotation direction
2) Cutter compensation C…………..Negative offset direction
3) Coordinate system rotation……………Negative rotation angle
4) Change the direction of the cutting feed
4.2.15
Coordinate System Rotation G68/G69
The machining workpiece consists of the figures by many same shapes, which can be
programmed by coordinate rotation function; only the subprogram should be programmed for the
figure unit, and then call the subprogram by the rotation function.
Code format:
G17 G68 X_ Y_ R_；
Or G18 G68 X_ Z_ R_；
Or G19 G68 Y_ Z_R_ ；
G69；
G17~G19：
Plane selection.
X_，Y_，Z_: Absolute command for two of the X_, Y_ and Z_ axes that
correspond to the current plane selected by a command (G17,
50
Chapter Four
Preparatory Function G Code
G18 and G19). The command specifies the coordinates of the
center of rotation for the values.
Specifying the axis commands (Y, Z, U, V, W, A, B and C) other than the X after the
G04 command, the system may alarm, and it is necessary to add the
absolute command explanation in the User Manual; specify the
rotation center followed with the G68.
R_：
Angle shifting, positive value means CCW.
Y
VOLUME I
PROGRAMMING
Rotation
angle
Rotation
center
X
Fig. 4-2-15-1
Function: The programmed shape inside the plane is rotated based upon that the specified center is
regarded as origin by the G68. G69 is used for cancelling the coordinate system rotation.
Explanations:
1. G68 can be held 2 positioning parameters, which are regarded as the optional parameters.
The positioning parameters are specified the center of the rotation operation. If the rotation
center does not specify, the system is regarded the current tool position as the rotation center.
The positioning parameters are related with the current coordinate plane, and select the X, Y
in the G17; Z,X in G18; Y, Z in G19.
2. The system is treated the specified point as the rotation center if the current positioning is
absolute method. The system is regarded the current point as the rotation center if the
positioning is relative method. G68, also, can be held a command parameter R, its parameter
value is the angle for the rotation, the positive value is CCW, and its rotation angle is degree.
The used rotation angle is determined by data parameter P329 when there is no rotation angle
in the coordinate rotation.
3. The system is regarded the current tool position as the rotation center in the G91 mode;
whether the rotation angle is performed the increment is set by the bit 0 of parameter No.: 47
(The rotation angle of coordinate, 0: Absolute code, 1: G90/G91 code).
4. The plane operation selection can not be performed when the system is on the rotation mode;
otherwise, the alarm occurs. It is necessary to note it when programming.
5. The G codes (G27～G30, etc.) of the reference point return and the G codes (G53～G59,
G54P1~G54P50, G9, etc.2) of command coordinate system can not be specified in the
51
GSK218MC Series Machining CNC System
Programming & Operation Manual
coordinate system rotation method. When, however, there is not alternative other than to
specify these G codes, it is better to specify it after the rotation function is cancelled; otherwise,
the system alarm may issue.
6. Perform the cutter compensation, tool length compensation, tool offset and other operations
after the coordinate system rotates.
7. Perform the coordinate rotation code in the scaling method (G51), the coordinate value of the
rotation center is also scaled instead of scaling the corner; when the movement code issues,
firstly perform the scaling and then rotate the coordinate.
Example 1: Rotation
G92 X-50 Y-50 G69 G17；
VOLUME I
PROGRAMMING
G68 X-50Y-50 R60；
G90 G01 X0 Y0 F200；
G91 X100；
G02 Y100 R100；
G3 X-100 I-50 J-50；
G01 Y-100；
G69；
M30；
Cutter path after rotating
The original
programming cutter path
（0，0）
60°
（-50，-50）
Rotation center
Fig. 4-2-15-2
Example 2: Scaling with rotation:
G51 X300 Y150 P0.5；
G68 X200 Y100 R45；
52
Chapter Four
Preparatory Function G Code
G01 G90 X400 Y100；
G91 Y100；
X-200；
Y-100；
X200；
G69 G50；
M30；
Only when the coordinate system
rotation function is performed
Y
When the scaling and
coordinate rotation
function are enabled.
VOLUME I
PROGRAMMING
Only when the scaling
function is performed.
200
Machined program
100
X
0
100
200
300
400
Fig. 4-2-15-3
Example 3： Repeatedly use the G68
According to the program (Main program)
G92 X0 Y0 Z20 G69 G17；
M3 S1000；
G0 Z2；
G42 D01；
(Tool offset setting)
M98 P2100(P02100)；
(Subprogram calling)
M98 P2200L7；
（Call for 7 times）
G40；
G0 G90 Z20；
X0Y0；
M30；
Subprogram 2200
O2200
G91
53
GSK218MC Series Machining CNC System
G68 X0 Y0 R45.0；
Programming & Operation Manual
(Relative rotation angle)
G90；
M98
P2100
；
(Subprogram O2200 calls the
subprogram O2100)
M99；
Subprogram 2100
Program path
（0，0）
O2100 G90 G0 X0 Y-20；
(Establish a right tool
The path with
offset value
（0，-20）
(14.142,-14.142)
compensation method)
VOLUME I
PROGRAMMING
G01Z－2 F200；
X8.284；
(8.284,-20)
Subprogram
X14.142 Y-14.142；
M99；
Fig. 4-2-15-4
4.2.16
Skip Function G31
Code format: G31 X_Y_Z_
Function: Linear interpolation can be commanded following the G31 code, like G01. If an external
skip signal is input during the execution of this code, and this execution of the code is then
interrupted and the next block is performed. The skip function is used when the end of the
machining is not programmed but specified with a signal from the machine, for example,
in grinding. It is used also for measuring the dimension of a workpiece.
Explanations:
1. G31 is one-shot mode G code, which is only enabled in the specified block.
2. The alarm occurs if the G31 code issues when the cutter compensation is applied; the
cutter compensation should be cancelled before G31 code.
Example:
The next block to G31 is 1 axis movement specified by an incremental value; refer to the Fig.
4-2-16-1:
54
Chapter Four
Preparatory Function G Code
Input the skip signal
50
Y
100
Actual movement
The movement
without skip signal
X
Fig. 4-2-16-1 The next block is 1 axis movement specified by an incremental value
VOLUME I
PROGRAMMING
The next block to G31 is 1 axis movement specified by an absolute value; refer to the Fig.
4-2-16-2:
Y100
G31 G90 X200 F100;
Y100;
Input the skip signal
Y
X200
Actual movement
The movement
without skip signal
X
Fig. 4-2-16-2 The next block is 1 axis movement specified by an absolute value
The next block to G31 is an absolute command for 2 axes; refer to the 4-2-16-3:
Y
100
Input the skip signal
(300,100)
Actual movement
The movement
without skip signal
X
100
200
300
Fig. 4-2-16-3 The next block is an absolute value for 2 axes
Note: It can be set by the bit 6 of parameter No.: 02 (SKIP signal, it is regarded as the signal input when 0 is
set to 1 and the 1 is set to 0).
55
GSK218MC Series Machining CNC System
4.2.17
Programming & Operation Manual
Inch/Metric Conversion (G20/G21)
Code format: G20: Inch input
G21: Metric input
Function: Either inch or metric can be carried out the program input.
Explanations:
Change the unit of the following values after the inch/metric is converted.
The feedrate, position code, workpiece zero offset value, tool compensation value, the scale
unit of MPG and the movement distance in the incremental feed are specified by F code.
When the power is turned on, the G code is the same as that held before the power was
turned off.
VOLUME I
PROGRAMMING
Notice: 1. The tool compensation value should be preseted based upon the least input incremental
unit when the inch shifts to metric or the metric converts into inch.
2. The 1st G28 code is identical with the same reference point return from the operation of the
intermediate point when the inch shifts to metric or the metric converts into inch.
3. When the least input incremental unit is different with the least command incremental unit,
the most error is an half of the least command unit, and this error does not accumulate.
4. Whether the program is input the inch or metric can be determined by the bit 2 of
parameter No.: 00.
5. Whether the program is output the inch or metric can be determined by the bit 0 of
parameter No.: 03.
6. It is essential to specify the G20 or G21 within the single block.
4.2.18
Optional Angle Chamfering/Corner Arc
Code format: , L_: Chamfering
, R_: Corner arc
Function: When the above-mentioned codes are added to the end of a block that specifies linear
interpolation (G10) or circular interpolation (G02, G03), a chamfering or corner arc is
automatically inserted during machining. Blocks specifying chamerfering and corner arc
can be specified consecutively.
Explanations:
1. After L, the chamfering specifies the distance from the virtual corner point to the start and
end points. The virtual corner point is the one that would exist if chamfering were not
performed; refer to the following figure:
56
Chapter Four
Preparatory Function G Code
（1）G91 G01 X100 ,L10;
（2）X100 Y100;
Insert the
chamfering block
L
L
Virtual center
Fig. 4-2-18-1
2. After R, specify the radius for corner arc, refer to the following figure:
VOLUME I
PROGRAMMING
（1）G91 G01 X100 ,R10;
（2）X100 Y100;
Arc center of radius R
R
Fig. 4-2-18-2
Restrictions:
1. Chamfering and corner arc only can be performed within the specified plane, and these
functions cannot be performed for parallel axes.
2. If the inserted chamfering or the block of the corner arc causes the tool to go beyond the
original interpolation movement range, the alarm is issued.
3. The corner arc can not be specified in the screw machining block.
4. When the specified chamfering value and the corner value are negative, the system is
assigned with the absolute value.
4.3
Reference Position G Code
The reference position is a fixed point on a machine tool to which the tool can be easily moved to
this point by the reference position function.
There are 3 code operation methods for the reference position, refer to the Fig. 4-3-1, the tool
can be automatically moved to the reference position along with the specified axis in code via an
intermediate point by G28; the tool can be automatically moved to the appointed point along with the
specified axis in code via an intermediate point by G29.
57
GSK218MC Series Machining CNC System
Programming & Operation Manual
Fig. 4-3-1
VOLUME I
PROGRAMMING
4.3.1
Format:
Reference Position Return (G28)
G28 X_ Y_ Z_
Function: G28 code is used for performing the operation, which returns to the reference position
(some one special position on the machine tool) by the intermediate point.
Explanation:
Intermediate point:
The intermediate point is specified by the code parameter in G28, which can be expressed by the
absolute value code or the incremental value code. The intermediate point coordinate value of the
code axis is registered during the execution of the block for supporting the G29 (return from the
reference position).
Notice:
The coordinate of the intermediate point is registered in the CNC, however, the coordinate value
of the axis specified by G28 is only registered each time. The other axes are not specified, which are
used the coordinate value specified by G28 before. And therefore, if you are not comprehend the
intermediate point in the default system when using the G28 command, it is better to specify each
axis. Consider it based upon the N5 block in the following example 1.
R (Reference position)
(3)
(2)
(1)
(4)
B
A
(5)
C
Fig. 4-3-1-1
1. The operation of the G28 block can be decomposed into following items (Refer to the Fig.
58
Chapter Four
Preparatory Function G Code
4-3-1-1):
(1) The current position positions to the intermediate point position (Point A → Point B) of
the command axis at the rapid traverse rate.
(2) Position to the reference position (Point B → Point R) from intermediate point at the
rapid traverse rate.
2. G28 is one-shot modal code, which is only enabled to the current block.
3. It is supported the referernce position return of the composition both the single or multi-axis.
The coordinate of the intermediate point is registered into CNC when the coordinate coordinate is
converted.
Example:
N1 G90 G54 X0 Y10；
Setting the intermediate point on X axis is X40 at the G54 workpiece
VOLUME I
PROGRAMMING
N2 G28 X40 ;
coordinate system, return to the reference point by (40, 10); that is, the X
axis is separately returned to the reference position.
N3 G29 X30 ;
Return to the (30, 10) via (40, 10) from reference; that is, the X axis is
returned to the destination alone.
N4 G01 X20；
N5 G28 Y60 ;
Intermediate point Y60。
N6 G55；
The workpiece coordinate system conversion, the intermediate point
changes into the point (40, 10) at the G55 coordinate system from the point
(40, 60) at the G54 workpiece coordinate system.
N7 G29 X60 Y20 ;
Reference position returns to the point (60, 20) via the intermediate point
(40, 60) at the G55 workpiece coordinate system.
G28 automatically cancels the tool compensations. This code, generally, is used
(Tool-change is performed at the reference position after returning the
reference point) in the automatical tool-change, therefore, when using
this code, it is necessary to cancel the cutter compensation and tool
length compensation firstly. Refer to the 1st reference position setting in
the data parameter P45～P48.
4.3.2
2nd, 3rd, and 4th Reference Position Retrun (G30)
Set 4 reference positions in the machine coordinate system. In a system without an
absolute-position detector, the 2nd, 3rd, and the 4th reference position return functions can be used
only after the automatical reference position return (G28) or the manual reference position return is
performed.
Format:
G30 P2 X_ Y_ Z_；the 2nd reference position return (P2 can be omitted)
59
GSK218MC Series Machining CNC System
Programming & Operation Manual
G30 P3 X_ Y_ Z_；the 3rd reference position return
G30 P4 X_ Y_ Z_；the 4th reference position return
Function: G30 performs the operation that the intermediate point specified in G30 returns to the
appointed reference position.
Explanations:
1. X_ Y_ Z_; Specify the code (Absolute value/incremental value code) at the intermediate
position
2. The setting and restriction of the G30 code are identical with the G28, the 2nd, 3rd, and the
4th reference position setting are shown the data parameters P50～P63.
3. G30 code can be used together with the G29 code (return from the reference position), and
its setting and restriction are same as the G28.
VOLUME I
PROGRAMMING
4.3.3
Automatically Return from Reference Position (G29)
Format: G29 X_ Y_ Z_
Function: G29 performs the operation that the appointed point returns from the reference position (or
current point) via the intermediate point specified by G28, G30.
Explations:
1. The motion of G29 block can be divided into the following steps (Refer to the Fig. 4-3-1-1):
(1) Positioning to the intermediate point (Point R → Point B) defined in G28, G30 from the
reference position (current point) at the rapid traverse rate.
(2) Positioning to the specified point (Point B → Point C) from a new intermediate point at
the rapid traverse rate.
2. G29 is one-shot modal information, which is only enabled for the current block. Generally, it is
necessary to immediately specify the code return from reference position following with the G28,
G30.
3. The optional parameters X, Y and Z in the G29 code format are used for specifying the
destination point (that is, the point C in Fig. 4-3-1-1) from the reference point return, which can be
indicated by an absolute value code or an incremental value code. For an incremental, the code
value specifies the incremental value departed from the intermediate point. When some axes are
not specified, that is, failure movement value relative to the intermediate point for these axes.
G29 is only followed by the command with one axis, which is the single axis return, the other
axes will invariable.
Example:
G90 G0 X10 Y10；
G91 G28 X20 Y20;
Return to the reference position via the intermediate point (30, 30)
G29 X30;
Return from the reference position (60, 30) via an intermediate point
(30. 30); it is note that it is in an incremental program method, and
60
Chapter Four
Preparatory Function G Code
the component along with the X axis direction is 60.
The intermediate point specified by G29 is assigned by G28, G30 code. For the definition of
the intermediate point, specification and system default, refer to the explantions in G28
code.
4.3.4
Reference Position Return Check (G27)
Format:
G27 X_ Y_ Z_
Function: G27 performs the reference position detection
Explanations:
the reference position return does not conduct. However, if the tool does not reach to the
reference position, the alarm occurs.
2. Machine tool locking state, that is, specify the G27 code, the tool is already returned to the
reference position automatically, and the completion signal return does not perform the breakover,
too.
3. In the offset mode, the tool arrived position is performed by G27 command, which is gained for
adding the offset value. Therefore, if the position adding to the offset value is not the reference
position, the signal does not conduct, and the alarm occurs. Usually, it is necessary to cancel the
tool offset before using the G27 code.
4. The X, Y or Z coordinate point position specified by G27 is the one below the machine tool
coordinate system.
4.4
Canned Cycle G Code
Canned cycle, is a machining operation, can be performed based upon multiple block codes by a
block with G function, so that the program can be simplified and the programming becomes easy for
the programmer (This system is only owned the canned cycle of the G17 plane).
The general procedure of canned cycle:
A canned cycle consists of a sequence of 6 operations; refer to the Fig. 4-4-1.
61
VOLUME I
PROGRAMMING
1. G27 code, tool positions at the rapid traverse rate. If the tool reaches to the reference position,
GSK218MC Series Machining CNC System
Operation 1
Programming & Operation Manual
Initial point
Operation 2
Operation 6
R
Operation 3
Operation 5
Rapid traverse
VOLUME I
PROGRAMMING
Operation 4
Cutting feed
Fig. 4-4-1
Operation 1: The positioning both the X axis and Y axis (Another axis is considered)
Operation 2: Move to the point R at a rapid traverse rate
Operation 3: Hole machining
Operation 4: The operation at the bottom of hole
Operation 5: Return to point R
Operation 6: Move to the initial point at a rapid traverse rate
Position in the XY plane, hole machining performs along with the Z axis. Specifying a canned
cycle operation is determined by 3 methods, which are separately specified by G codes.
1) Data form
G90 absolute value method;
G91 Incremental value method
2) Return to the point plane
G98 Initial point plane;
G99 Point R plane
3) Hole machining method
G73, G74, G76, G81～G89
Plane both in initial point Z and point R
Initial point plane: Tool’s absolute position along with the Z axis direction before the canned
cycle state.
Point R plane: It is also called Safety Plane, which is the position along with the Z axis direction
in the canned cycle when the rapid traverse turns into cutting feed. Generally,
position at some certain distance above a workpiece surface to prevent the tool
from impacting to the workpiece; and guard the adequate distance to complete
the acceleration procedure.
G73/G74 /G76/G81～G89 are specified the overall data (hole position data, hole machining data,
repeated times) of the canned cycle to compose a block.
Z, R: Either the parameter Z at the bottom of a hole or the parameter R may be absent when
62
Chapter Four
Preparatory Function G Code
performing the 1st drilling hole; the system is only altered the modal and performed the Z axis
operation.
The format of the hole machining method is as follows:
（G17） G__
X__ Y__ Z__ R__ Q__ P__ F__ K__;
Hole machining data
Hole position data
Hole machining method
Wherein, the basis meanings of hole position data and hole machining data are shown in the
table 4-4-1:
VOLUME I
PROGRAMMING
Table 4-4-1
Specified
Parameter
content
word
Explanation
Hole
machining
G
Refer to the table 4-4-3, note above-mentioned restrictions
method
Hole
position
X，Y
data
Specify the hole position by an absolute value or an
incremental value; the control is same as the G00 positioning.
Figure 4-4-2 shows that the incremental value specifies the
distance to the bottom of a hole from point R or the absolute
Hole
machining
value commands the coordinate value at the bottom of a hole.
Z
data
Refer to the feedrate in the Fig. 4-4-1, the feedrate is
specified by F in operation 3; in the operation 5, it is the rapid
traverse rate or the feedrate by F code based upon different
hole machining methods.
The figure 4-4-2 shows that the distance from initial point
plane to point R is specified by incremental value, or the
R
coordinate value of the point R is specified by absolute value.
The feedrate, in the operations 2 and 6, are performed at the
rapid traverse rate; refer to the Fig. 4-4-1.
Q
Specify the cutting value for each time in G73, G83 or the
translation value (incremental value) in G76, G87.
63
GSK218MC Series Machining CNC System
Specified
Parameter
content
word
Programming & Operation Manual
Explanation
Specify a dwell time at the bottom of a hole. A canned cycle
codes can be accompanied a parameter P_, in the P_
P
parameter value, perform the dwell operation time after the
specified tool reaches to the plane Z; its unit is ms. The least
value of parameter is determined by P281, and its most value
is set by P282.
F
Specify the cutting feedrate
Change only the modal.
Specify the repeated time in the K_ parameter value, and the
VOLUME I
PROGRAMMING
K is only enabled with the specified block. If it omits, it regards
K
as once bey default. The maximum drilling times is 99999;
when the negative value is specified, and then perform it base
upon the absolute value; when it is 0, the drilling hole
operation is omitted.
Restrictions:
¾ Canned cycle G code is the modal one, which always keeps enabling until the G code of the
specified canned cycle is cancelled.
¾ The G80 and the G code of group 01 is cancelled the G code of canned cycle.
¾ Machining data is always performed till the end of the canned cycle once it is specified in a
canned cycle; therefore, the necessary hole machining data should be specified at the
beginning of the canned cycle, and only the altered data should be specified in the following
canned cycle.
Note 1: The cutting feedrate specified by F is held even if the canned cycle is cancelled.
Note 2: the scaling function along Z axis (cutting axle direction) is disabled when the canned cycle is performed.
Note 3: In the single mode, the canned cycle mostly uses 3 sections machining methods: positioning → R plane →
Initial plane.
Note 4: In the canned cycle, when the bit 1 of parameter No.: 36 is set to 1, the hole machining data and the hole
position data are eliminated in the REST or ESP. The examples of data hold and clean in the above-mentioned
are shown below:
Table 4-4-2
Sequence
64
Data
Explanation
specification
①
G00X_M3；
②
G81X_Y_Z_R_F_;
Specify the required value for the Z, R and F because it is at the
beginning.
Chapter Four
③
Y_;
Preparatory Function G Code
G81 and Z-R-F- can be omitted because the hole machining
method specified in hole ② is identical with the hole machining
data. The position movement Y of a hole is machined once by G81
method.
④
G82X_P_;
It is only moved along with X axis relative to the hole ③. Machining
is performed by G82, and the hole machining data is performed by
the Z, R and F specified in ② and the P specified in ④.
G80X_ Y_
Do not perform the hole machining. Cancel the overall hole
machining data.
Z and R should be specified again because the overall data are
⑥
G85X_Z_R_P_;
cancelled in ⑤.
F can be omitted because it is same with the specified one in ②.
P, is unavaliable in this block, is only saved.
⑦
X_Z_;
For ⑥, it is the hole machining with the different Z values, and the
hole position is only enabled moved along with X axis.
The specified Z in ⑦, the R, P in ⑥ and the F in ② are regarded as
⑧
G89X_Y_;
the hole machining data, and perform the hole machining for G89
method.
⑨
G01X_Y_;
Eliminate the hole machining method and data
A. The absolute value code and incremental value code G90/G91 of canned cycle
The G90 and G91 are changed along with the distance of the drilling axis; refer to the Fig. 4-4-2.
(Generally, program is performed using G90; if the G91 is used, the Z and R will be treated based
upon the +/- of the command)
65
VOLUME I
PROGRAMMING
⑤
GSK218MC Series Machining CNC System
G90 (Absolute command)
Programming & Operation Manual
G91 (Incremental command)
Z=0
Z=0
R
Point R
R
Z
Point R
Z
Point Z
Point Z
Relative
Absolute
VOLUME I
PROGRAMMING
(A)
(B)
Fig. 4-4-2
B. The plane return code G98/G99 of canned cycle
Tool can be returned to the point R plane or initial position plane after the tool is arrived to the
bottom of a hole. The tool can be returned to the initial point plane or point R plane based upon the
different of G98 and G99.
Usually, the G99 is used for drilling at the 1st time and the G98 is at the last. The initial plane
invarible even if the machining is performed by G99. The operations of G98 and G99 are shown
below:
G98 is regarded as the system default.
G98 (Return to the initial
point plane)
G99 (Return to the point
R plane)
Initial point
plane
Initial point
plane
Point R
Fig. 4-4-3
The explanation symbols of each canned cycle, refer to the following figure.
66
Chapter Four
Preparatory Function G Code
Positioning (rapid
traverse G0)
Cutting feed (linear
interpolation G1)
Manual feed
Offset (rapid traverse G0)
P
Dwell
Fig. 4-4-4
The comparison table (G73～G89) of canned cycle
G code
Drilling
Operation at the
Retraction
(-Z direction)
bottom of a hole
(+ Z direction)
G73
Intermittent feed
G74
Feed
G76
Feed
Dwell-spindle
positive
Oriented spindle
stop
Application
Rapid traverse
High-speed peck machining
Rapid traverse
Counter-tapping cycle
Rapid traverse
Fine boring cycle
G80
Canned cycle cancel
G81
Feed
G82
Feed
G83
Intermittent feed
G84
Feed
G85
Feed
G86
Feed
G87
Feed
G88
Feed
G89
Feed
Rapid traverse
Drilling, spot drilling
Rapid traverse
Drilling, bore the stage hole
Rapid traverse
Peck machining cycle
Feed
Tapping
Feed
Boring
Spindle stop
Rapid traverse
Boring
Spindle positive
Rapid traverse
Boring
Dwell → spindle
Manual → spindle
stop
positive
Dwell
Feed
Dwell
Dwll Š spindle
negative
Boring
Boring
Restriction:
Tool radius offset (D) will be omitted during the canned cycle positioning.
67
VOLUME I
PROGRAMMING
Table 4-4-3
GSK218MC Series Machining CNC System
4.4.1
Programming & Operation Manual
High-speed Peck Machining Cycle G73
Code format:
G73 X_Y_Z_R_Q_F_K_
Function: This cycle is specially set for performing the high-speed peck drilling, which is performed
the intermittent cutting feed till to the bottom of a hole; simultaneously, it retreats from the
hole at the rapid traverse during feed, and then eliminate the cutting chip. The operation
schematic shows in the figure 4-4-1-1.
Explanations:
X_Y_: Hole position data;
Z_: Incremental programming means specify the distance form point R to the bottom of a hole;
absolute programming means the absolute coordinate value at the bottom of a hole;
VOLUME I
PROGRAMMING
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of the point R;
Q_ Depth of cut for each cutting feed;
F_: Cutting feedrate
K_: Number of repeats.
G73（G98）
G73（G99）
Initial point
plane
Point R plane
R
q
q
R
q
d
q
d
q
d
d
q
Z
Z
Fig. 4-4-1-1
Z, R: Parameters both the Z and R at the bottom of a hole will be simultaneously absented when
performing the 1st drilling, and then the system executes the operation along Z axis.
Q: When the code parameter Q is specified, the above-mentioned intermittent feed is then
performed. In this case, the system is retracted based upon the clearance d (Fig. 4-4-1-1) set in the
data parameter P270. Each time for feed, the tool intermittently performs the retraction of that
distance d at the rapid traverse rate.
When the G73 code and an M code are specified in the same block, the M code is executed at
the time of the first positioning operation. The system then proceeds to the next drilling operation.
68
Chapter Four
Preparatory Function G Code
When K is used to specify the number of repeats, the M code is executed for the first hole only;
for the second and subsequent holes, the M code is not executed.
Note 1: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Note 2: When the bit 1 of parameter No.:43 is 0 and there is no cutting value in peck drilling (G73, G83), the alarm
does not issue; in this case, fail to specify the code parameter Q or the Q is set to 0, the system performs the
hole position at the X, Y plane instead of executing the drilling operation. When the bit 1 of parameter No.: 43 is
1, the alarm generates if there is no cutting value in peck drilling (G73, G83); that is, fail to specify the code
parameter Q or the Q is set to 0; the system alarm prompts: “0045: fail to find address Q or the Q value is 0
(G73/G83)”. If the Q value is specified as negative, the system then performs the intermittent feed based upon
the absolute value.
Note 3: Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded a same block
modal, if the tool compensation G43, G44 or G49 is placed at one block separately, the system is then
performed the offset value addition or cancellation with real-time.
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G73 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Example:
M3 S1500；
Cause the spindle to start rotating.
G90 G99 G73 X0 Y0 Z-15 R-10 Q5 F120； Position, drill hole 1, then return to point R
Y-50；
Position, drill hole 2, then return to point R
Y-80；
Position, drill hole 3, then return to point R
X10；
Position, drill hole 4, then return to point R
Y10；
Position, drill hole 5, then return to point R
G98 Y75；
Position, drill hole 6, then return to the initial level
G80；
G28 G91 X0 Y0 Z0；
Return to the reference position
M5；
Spindle rotation stop
M30；
Note: When the 2～6 hold machining are performed in the above-mentioned example; although the Q is omitted, the
chip-removal operation still performs.
4.4.2
Drilling Cycle, Spot Drilling Cycle (G81)
Code format: G81 X_ Y_ Z_ R_ F_ K_
69
VOLUME I
PROGRAMMING
with the canned cycle, add or cancel an offset value at the time of positioning to point R; in the canned cycle
GSK218MC Series Machining CNC System
Programming & Operation Manual
Function: This cycle is used for normal drilling cutting feed and performed to the bottom of the hole.
The tool is then retreated from the bottom of the hole at the rapid traverse rate.
Explanations:
X_Y_: Hole position data;
Z_: Incremental program means specify the distance form point R to the bottom of a hole;
absolute program means the coordinate value at the bottom of a hole;
R_: Incremental program means the distance from the initial point plane to the point R;
absolute program means the coordinate value of the point R;
F_: Cutting feedrate
K_: Number of repeats (if required).
VOLUME I
PROGRAMMING
G81（G98）
G81（G99）
Initial point plane
Point R plane
Point R
Point R
Point Z
Point Z
Fig. 4-4-2-1
Z, R: Either parameter Z or R at the bottom of a hole may be absent when performing the 1st drilling,
the system changes the modal only instead of performing the operation along with Z axis.
Rapidly move to the point R after positioning along with the X and Y axes, perform the drilling
machining from the point R to Z, and then tool retracts at the rapid traverse rate.
Rotate the spindle with the miscellaneous function M code before specifying the G81.
When the G81 code and an M code are specified in the same block, the M code is executed at
the time of the first positioning operation. The system then proceeds to the next drilling operation.
When K is used to specify the number of repeats, the M code is executed for the first hole only;
for the second and subsequent holes, the M code is not executed.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
70
Chapter Four
Preparatory Function G Code
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
Example:
M3 S2000
Spindle rotation
G90 G99 G81 X300 Y-250 Z-150 R-10 F120; Positioning, drill hole 1, then return to point R
Y-550.；
Positioning, drill hole 2, then return to point R
Y-750.；
Positioning, drill hole 3, then return to point R
X1000.；
Positioning, drill hole 4, then return to point R
Y-550.；
Positioning, drill hole 5, then return to point R
G98 Y-750.；
Positioning, drill hole 5, then return to initial position plane
VOLUME I
PROGRAMMING
G80；
G28 G91 X0 Y0 Z0 ；
M5；
Return to the reference position
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G81 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.4.3
Drilling Cydle, Counter Boring Cycle (G82)
Code format: G82 X_ Y_ Z_ R_ P_ F_ K_；
Function: This cycle is used for normal drilling. Butting feed is performed to the bottom of the hole. At
the bottom, a dwell is performed, then the tool is retracted in rapid traverse.
Explanations:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance of the specified point R to the bottom of a
hole; absolute programming means the absolute coordinate value of the bottom of a hole;
R_: Incremental programming means the distance from the initial point plane to point R;
absolute programming means the absolute coordinate value of point R;
F_: Cutting feedrate;
P_: Dwell time at the bottom of a hole;
K_: Repeated times.
71
GSK218MC Series Machining CNC System
G82（G98）
Programming & Operation Manual
G82（G99）
Initial point plane
Point R plane
R
R
VOLUME I
PROGRAMMING
P
P
Z
Z
Fig. 4-4-3-1
After positioning along the X and Y axes, rapid traverse is performed to point R. Drilling is then
performed from point R to Z. when the bottom of the hole has been reached, a dwell is performed.
The tool is then retracted in rapid traverse.
The miscellaneous function M code rotates the spindle before specifying G82.
When the G82 and M codes are specified in the same block, the M code is executed at the time
of the 1st positioning operation. The system then proceeds to the next drilling operation.
When the repeated times K is specified, the M code is executed for the 1st hole only instead of
performing the second and subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
P is the modal code, the least value of parameter is set by data parameter P281 and the most
value is set by p282. Value P is less than the P281 parameter setting value, which is operated based
upon the least value; if it more than the P282 parameter setting value and it is operated based upon
the most value.
Example:
M3 S2000 Spindle rotation
G90 G99 G82 X300 Y-250 Z-150 R-100 P1000 F120； Positioning, drill hole 1, dwell for 1s at
thebottom of the hole, then return to the point R
Y-550；
72
Positioning, drill hole 2, dwell for 1s at thebottom of the hole, then return to the point R
Chapter Four
Y-750；
Preparatory Function G Code
Positioning, drill hole 3, dwell for 1s at thebottom of the hole, then return to the point R
X1000.； Positioning, drill hole 4, dwell for 1s at thebottom of the hole, then return to the point R
Y-550；
Positioning, drill hole 5, dwell for 1s at thebottom of the hole, then return to the point R
G98 Y-750；
Positioning, drill hole 1, dwell for 1s at thebottom of the hole, then return to the
initial position plane
G80；
Canned cycle cancellation
G28 G91 X0 Y0 Z0 ；
Reference position return
M5；
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
otherwise, the G60 is replaced by G82.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.4.4
Peck Drilling Cycle (G83)
Code format:
G83 X_ Y_ Z_ R_ Q_ F_ K_
Function: This cycle performs peck drilling. It performs intermittent cutting feed to the bottom of a
hole while removing shavings from the hole.
Explanations:
X_Y_: Hole position data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value of the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of the point R;
Q_: Cutting depth of each cutting feed;
F_: Cutting feedrate;
K_: Repeated times.
73
VOLUME I
PROGRAMMING
parameter No.:48 is set to 1)) of group 01 in a same block when using G81 command;
GSK218MC Series Machining CNC System
G83（G98）
Programming & Operation Manual
G83（G99）
Initial point plane
Point R plane
R
q
q
q
d
d
q
d
d
VOLUME I
PROGRAMMING
Z
Z
Fig. 4-4-4-1
Q: It represents the depth of cut for each cutting feed. It must always be specified as an
incremental value. In the second and subsequent cutting feeds, rapid traverse is performed up to
a point d just before where the last drilling ended, and the cutting feed is performed again. The
value of d is set by parameter P271 as the Fig. 4-4-4-1 shows.
Be sure to specify a positive value in Q. Negative values are ignored and the system is still
treated by positive.
Specify Q in the block of drilling, if it is not specified in the block without drilling; Q is registered as
the modal data.
Use a miscellaneous function to rotate the spindle (M code) before specifying G83.
When G83 and M codes are specified in the same block, the M code is executed at the time of
the 1st hole positioning operation. The system then proceeds to the next drilling operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note 1: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Note 2: When the bit 1 of parameter No.:43 equals to 0, there is no alarm without specifying the cutting value in peck
drilling (G73, G83), in this case, the Q does not specify or sets to 0; the system performs the hole positioning
along with X, Y plane instead of executing the drilling operation. When the bit 1 of parameter No.:43 equals to 1,
the alarm occurs without specifying the cutting value in peck drilling (G73, G83); that is, the code parameter Q
does not specified or sets to 0; the system alarms: “0045: the address Q does not find or sets to 0 (G73/G83)”. If
the Q value is specified as negative, the system then performs intermittent feed based upon its absolute value.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
74
Chapter Four
Preparatory Function G Code
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
Example:
M3 S2000；
Spindle rotation
G90 G99 G83 X300 Y-250 Z-150 R-100 Q15 F120; Positioning, drill hole 1, then return to point R
Y-550；
Positioning, drill hole 2, then return to point R
Y-750；
Positioning, drill hole 3, then return to point R
X1000；
Positioning, drill hole 4, then return to point R
Y-550；
Positioning, drill hole 5, then return to point R
Positioning, drill hole 5, then return to initial position plane
G80；
G28 G91 X0 Y0 Z0 ；
Reference position return
M5；
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G83 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.4.5
Tapping Cycle G74 (or G84)
Code format:
G74/G84 X_ Y_ Z_ R_ P_ F_K_
Function: This cycle performs tapping. In the tapping cycle, the dwell is performed when the tapping axis
reaches to the bottom of the hole, then the spindle retracts the tapping axis with the negative
rotation. (G74 is left-counter tapping cycle, G84 is right-counter tapping)
Explanations:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
P_: Dwell time at the bottom of a hole;
F_: Tapping feedrate;
K_: Repeated times; (if required)
75
VOLUME I
PROGRAMMING
G98 Y-750；
GSK218MC Series Machining CNC System
G74（G98）
Programming & Operation Manual
G74（G99）
Initial point plane
Point R plane
Spindle
positive
R
Spindle
positive
R
P
P
Spindle
negative
Spindle
negative
VOLUME I
PROGRAMMING
P
P
Z
G84（G98）
Z
G84（G99）
Initial point plane
Point R plane
Spindle
negative
R
Spindle
negative
R
P
P
Spindle
positive
Spindle
positive
P
P
Z
Z
Fig. 4-4-5-1
When specifying the G74, spindle performs the tapping CW (When specifying G84, the spindle is
CCW); the dwell is performed when it reaches to the bottom of the hole, then the spindle is rotated
along with a reverse direction; simultaneously, the feedrate specified by program retracts the tapping
axis, so that the screw occurs.
Example:
G94
Feed/min.;
M29 S1000 ；
Spindle exact stop, specify the spindle speed;
G43 / G44 H10 ；
Call the tool length compensation
G90 G99 G74 / G84 X100 Y110 Z -50 R5 P3000 F100； Positioning, tapping hole 1, then return
topoint R;
Y150；
76
Positioning, tapping hole 2, then return topoint R;
Chapter Four
Preparatory Function G Code
G91 X50 K5；
It performs along with X axis based upon the
reference point X100, Y150
50mm means that the incremental unit performs the tapping for 5 times;
G98 Y-750；
Positioning, tapping hole 8, then return to the initial point;
G80；
Cancel the tapping cycle;
G28 G91 X0 Y0 Z0 ；
return to the reference position;
M30；
End of program;
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded a
same block with the canned cycle, add or cancel an offset value at the time of
positioning to point R; in the canned cycle modal, if the tool compensation G43, G44
value addition or cancellation with real-time.
Screw leading: In the feed/min. mode, the relationships among the screw leading, feedrate and
spindle speed are shown below:
Feedrate F = screw tap pitch × spindle speed S
For example: tap the M12×1.5 screw hole in component, optional parameter;
S500=500ｒ/min；
F=1.5×500=750mm/min；
In multiple thread, the F value can be calculated by multiplying by the numbers of
thread head.
In feed/rev. mode, the thread leading equals to the feedrate.
Example:
Feed/min.：
Feed/rev.:
Spindle speed 1000r/min；
Spindle speed 1000r/min；
Thread leading 1.0mm；
Thread leading
1.0mm；
Then, Z axis feedrate= 1000*1=1000mm/min; Then, Z axis feedrate= thread leading =1mm / r;
G94
Feed/min.
G95
Feed/rev.
G00 X120 Y100 ;
Positioning
G00 X120 Y100；
Positioning
M29 S1000 ;
Rigid method
M29 S1000 ；
Rigid method
G84 Z-100 R-20 F1000; Right-counter rigid tapping G84 Z-100 R-20 F1;Right-counter rigid
tapping
G80
Tapping cycle cancellation
G28 G91 X0 Y0 Z0 Reference point return
M30
End-of-program
G80
Tapping cycle cancellation
G28 G91 X0 Y0 Z0
M30
Reference point return
End-of-program
Restrictions:
G code:
When using the G74/G84 command, fail to specify G code in 01 (G00 to G03, G60 is
77
VOLUME I
PROGRAMMING
or G49 is placed at one block separately, the system is then performed the offset
GSK218MC Series Machining CNC System
Programming & Operation Manual
modal code (bit 0 of parameter No.:48 sets to 1)) group at the same block, the system then
shifts to the G60 modal.
When the G74/G84 and M codes are specified at a same block, perform the M code
while the 1st hole is performed the positioning operation; the next tapping operation is
then disposed.
M code:
To use the miscellaneous function M code rotates the spindle before specifying the
G74/G84. If the spindle rotation does not specify, the system automatically rotates based
upon the current spindle command speed in the R plane, then adjust as the CW
(G74)/CCW (G84). When the G74/G84 and the M code are specified at a same block,
perform the M code at the time of performing the 1st hole position operation. The system
then proceeds next tapping.
VOLUME I
PROGRAMMING
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the
program; perform the above-mentioned M code after executing the current statement.
S command:
If the specified spindle speed exceeds the top spindle speed in tapping (data
parameter P257: the upper limit speed of spindle in tapping cycle), the system then
alarms; the top speed level of the spindle in the rigid tapping is determined by
P94~P296.
F command: If the specified F value exceeds the upper limit value of the cutting feedrate (data
parameter: P96 sets the upper limit value), it is subject to the upper limit value.
P command: P is the modal code, the minimum value of parameter is set by data parameter P281;
the maximum value of parameter is determined by data parameter P282. P is oprated
based upon the minimum value when it is less than the parametr setting value of
P281 and it is operated based upon the maximum value when it is more than the
parameter setting value of P282.
Axis shifting: Cancel the canned cycle before shifting the tapping axis. If the tapping axis is changed
in rigid tapping mode, the system then shows the No.206 alarm.
Override: The feedrate and spindle rotation feedrate are 100% by default during the tapping; the
machine tool still operates after pressing the feed hold button till the completion of the
operation return.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Program restart: The program restart function is disabled in tapping cycle.
78
Chapter Four
4.4.6
Preparatory Function G Code
Fine Boring Cycle (G76)
G76 X_Y_Z_Q_R_P_F_K_
Code format:
Function: The fine boring cycle is available for a hole with fine boring.
When reaching to the bottom of the hole, the spindle stops, and the tool is moved away from
the machined surface of the workpiece and retracted.
To prevent the tool retraction path during retreating from impacting the smoothness on the
machining surface, simultaneously, to avoid the damage of the tool.
Explanations:
X_Y_: Hole position data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
Q_: Offset value at the bottom of a hoel
P_: Dwell time at the bottom of a hole;
F_: Cutting feedrate;
K_: Times of the fine boring.
G76（G98）
Spindle
positive
Spindle exact
stop
Initial point
plane
G76（G99）
Spindle
positive
Point R plane
tool
R
R
Spindle
exact stop
P
Translation value q
q
Z
Rapid
traverse (G0)
Spindle
exact stop
P
q
Z
Rapid
traverse (G0)
Fig. 4-4-6-1
The spindle stops on the canned revolving position when the tool reaches to the bottom of a hole,
and tool moves and retracts based upon the reverse direction of tool nose. So that the machining
surface will not be damage, and then the precise and enabled boring machining can be carried out.
Parameter Q specifies the distance of tool-retraction. The tool-retraction direction and its axis can be
specified by the bit 4 and 5 of parameter No.: 42; the Q value should be positive; and the sysmbol is
still disabled even if using the negative. The offset value of the Q at the bottom of a hole is the
79
VOLUME I
PROGRAMMING
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
GSK218MC Series Machining CNC System
Programming & Operation Manual
registered modal value within the canned cycle, so it is important to specify it carefully. And therefore,
it also uses for cutting depth of the G73 and G83.
To use the miscellandous function M code rotates the spindle before specifying the G76.
When the G74 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation. The system then proceeds the next operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is
commanded a same block with the canned cycle, add or cancel an offset value at the time of
VOLUME I
PROGRAMMING
positioning to point R; in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed
at one block separately, the system is then performed the offset value addition or cancellation with
real-time.
Axis shifting: Cancel the canned cycle before altering the drilling axis.
Boring machining: Fail to perform the boring maching in the block without X, Y and Z or othere
axes.
Example:
M3 S500；Spindle rotation
G90 G99 G76 X300 Y-250 Z-150 R-100 Q5 P1000 F120; Positioning, bore hole 1, then return to
point R, move 5mm when the
orientation is performed at the bottom
of ahole, and stops 1s.
Y-550； Positioning, bore hole 2, then return to point R
Y-750； Positioning, bore hole 3, then return to point R
X1000；Positioning, bore hole 4, then return to point R
Y-550； Positioning, drill hole 5, then return to point R
G98 Y-750； Positioning, bore hole 6, and then return to the initial position plane
G80 G28 G91 X0 Y0 Z0; Return to the reference point
M5；Spindle stop
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G76 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Note 1: The in-feed axis and the in-feed direction are canned in this command, and the in-feed direction is regardless
of the rotation of the G68 coordinate system.
80
Chapter Four
4.4.7
Preparatory Function G Code
Boring Cycle (G85)
Code format: G85 X_ Y_ Z_ R_ F_ K_
Function: This cycle is used to bore a hole.
Explanations:
X_Y_: Hole position data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
F_: Cutting feedrate;
G85（G98）
VOLUME I
PROGRAMMING
K_: Repeated times.
G85（G99）
Initial point
plane
Point R plane
R
R
Z
Z
Fig. 4-4-7-1
Rapid traverse to point R after positioning along the X and Y axes, and then perform a boring
from point R to Z; perform the cutting feed to return point R when reaching to the bottom of a hole.
Before specifying G85, use a miscellaneous function (M code) to rotate the spindle.
When the G85 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation. The system then proceeds the next operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
81
GSK218MC Series Machining CNC System
Programming & Operation Manual
separately, the system is then performed the offset value addition or cancellation with real-time.
Axis switching: Cancel the canned cycle before the drilling axis can be changed.
Boring machining: In a block that does not contain X, Y, Z or other axes is not performed.
Example
M3 S100 ；
Spindle rotation
G90 G99 G85 X300 Y-250 Z-150 R-120 F120； Positioning, bore hole 1, then return to point R
Y-550；
Positioning, bore hole 2, then return to point R
Y-750；
Positioning, bore hole 3, then return to point R
X1000；
Positioning, bore hole 4, then return to point R
Y-550；
Positioning, bore hole 5, then return to point R
VOLUME I
PROGRAMMING
G98 Y-750；
Positioning, bore hole 6, and then return to the initial position plane.
G80；
G28 G91 X0 Y0 Z0 ；
Return to reference point
M5；
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G85 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.4.8
Boring Cycle (G85)
Code format:
G86 X_ Y_ Z_ R_ F_ K_；
Function: This cycle code is used for boring machining cycle. (omit the dwell operation at the bottom
of a hole)
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
F_: Cutting feedrate;
K_: Repeated machining times.
82
Chapter Four
Preparatory Function G Code
G86（G98）
G86（G99）
Spindle positive
Initial point
plane
Spindle
positive
R
R
Point R
plane
Z
Z
Fig. 4-4-8-1
Rapid traverse to point R after positioning along the X and Y axes, and then perform a boring
from point R to Z; tool retracts at a rapid traverse rate when reaching to the bottom of a hole.
Before specifying G86, use a miscellaneous function (M code) to rotate the spindle.
When the G86 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation, and then, the system then proceeds the next operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only instead fo
performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
Axis switching: Cancel the canned cycle before the drilling axis can be changed.
Boring machining: In a block that does not contain X, Y, Z or other axes is not performed.
For example:
M3 S2000；
Spindle rotation
G90 G99 G86 X300 Y-250 Z-150 R-100 F120
Positioning, bore hole 1, then return to point R
Y-550；
Positioning, bore hole 2, then return to point R
Y-750；
Positioning, bore hole 3, then return to point R
X1000；
Positioning, bore hole 4, then return to point R
Y-550；
Positioning, bore hole 5, then return to point R
G98 Y-750；
Positioning, bore hole 5, then return to the initial position plane
83
VOLUME I
PROGRAMMING
Spindle
stop
Spindle
stop
GSK218MC Series Machining CNC System
Programming & Operation Manual
G80；
G28 G91 X0 Y0 Z0 ；
Return to the reference point
M5；
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G86 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
VOLUME I
PROGRAMMING
4.4.9
Hole Cycle, Back Boring Cycle (G87)
Code format:
G87
X_Y_Z_R_Q_P_ F_；
Function: This cycle performs accurate boring
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R; (the bottom of the hole)
Q_: Offset value at the bottom of a hole
P_ Dwell time at the bottom of a hole;
F_: Cutting feedrate;
84
Chapter Four
Preparatory Function G Code
G87（G98/G99）
Spindle
exact stop
Initial point
plane
Spindle
positive
Spindle
exact stop
Spindle Z
exact stop
tool
P
q
R
Rapid
traverse (G0)
Translation value q
Fig. 4-4-9-1
Spindle stops the tool after orientation along with the X and Y axes and moves at the opposite
direction along the tool nose, and movement is performed to the bottom of the hole (point R). The tool
is then shofted in the direction of tool nose and the spindle is rotated negatively. Boring is performed
in the positive direction along the Z axis until the point Z is reached. At point Z, the spindle is stopped
at the fixed rotation position again, the tool is shifted in the direction opposite to the tool tip, then the
tool is returned to the initial level. The tool is then shifted in the direction of the tool tip and the spindle
is rotated CW to proceed to the next block operation.
Parameter Q specifies the distance of tool-retraction. The tool-retraction direction and its axis
can be specified by the bit 4 and 5 of parameter No.: 42; the Q value should be positive; and the
sysmbol is still disabled even if using the negative. The offset value of the Q at the bottom of a hole is
the registered modal value within the canned cycle, so it is important to specify it carefully. And
therefore, it also uses for cutting depth of the G73 and G83.
Before specifying G87, use a miscellaneous function (M code) to rotate the spindle.
When the G87 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation, and then, the system then proceeds the next tapping.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
85
VOLUME I
PROGRAMMING
Spindle
negative
GSK218MC Series Machining CNC System
Programming & Operation Manual
separately, the system is then performed the offset value addition or cancellation with real-time.
Canned cycle is only performed on the G17 plane.
Boring machining: Fail to perform the boring machining in the block without the X, Y, Z or other
miscellaneous axis.
Prompt: When performing the back boring cycle, it is necessary to remember that the values Z and R
should be specified. Generally, the position Z is above the position R; otherwise, the system
alarm may occur.
Example:
M3 S500；Spindle rotation
G90 G99 G87 X300 Y-250 Z-120 R-150 Q5 P1000 F120；
(Positioning, bore hole 1, positioning at the initial position and then offset 5mm to stop at point Z
VOLUME I
PROGRAMMING
for 1 second)
Y-550；
Positioning, bore hole 2, then return to initial position plane
Y-750；
Positioning, bore hole 3, then return to initial position plane
X1000；
Positioning, bore hole 4, then return to initial position plane
Y-550；
Positioning, bore hole 5, then return to initial position plane
G98 Y-750；
Positioning, bore hole 6, then return to initial position plane
G80 G28 G91 X0 Y0 Z0 ； Return to the reference point
M5；
Spindle rotation stop
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G87 command;
otherwise, the G87 is replaced by G code of group 01.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Note 1: In this command, in-feed axis and direction are fixed, and the in-feed direction is regardless of the rotation of
the G68 coordinate system.
4.4.10
Boring Cycle (G88)
Code format: G88
X_Y_Z_R_ P_F_
Function: This cycle is used for boring a hole.
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
86
Chapter Four
Preparatory Function G Code
P_ Dwell time at the bottom of the hole;
F_: Cutting feedrate.
G88（G98）
G88（G99）
Spindle
positive
Initial point
plane
Spindle
positive
R
R
Point R plane
VOLUME I
PROGRAMMING
Spindle
stop
Spindle
stop
Z
Z
Fig. 4-4-10-1
Rapidly move to point R, and then the boring is performed from point R to Z after positioning is
carried out along with the X and Y axes. Dwell is performed after the boring is executed, the the
spindle stops; tool returns to the point R (G99) or initial point (G98) manually from the point Z where
places at the bottom of the hole, and then spindle rotates positively.
Before specifying G88, use a miscellaneous function (M code) to rotate the spindle.
When the G88 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation, and then, the system then proceeds the next drilling
operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
P is the modal code, the least value of parameter is set by data parameter P281 and the most
value is set by p282. Value P is less than the P281 parameter setting value, which is operated based
upon the least value; if it more than the P282 parameter setting value and it is operated based upon
the most value.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
Axis switching: Cancel the canned cycle before the boring axis can be shifted.
Boring machining: In a block that does not contain X, Y, Z or other miscellaneous axes is not
87
GSK218MC Series Machining CNC System
Programming & Operation Manual
performed.
Example:
M3 S2000；
Spindle rotation
G90 G99 G88 X300 Y-250 Z-150 R-100 P1000 F120； Positioning, bore hole 1, then return to point R
Y-550；
Positioning, bore hole 2, then return to point R
Y-750；
Positioning, bore hole 3, then return to point R
X1000；
Positioning, bore hole 4, then return to point R
Y-550；
Positioning, bore hole 5, then return to point R
G98 Y-750；
Positioning, bore hole 6, then return to initial
VOLUME I
PROGRAMMING
position plane
G80 G28 G91 X0 Y0 Z0；
Return to the reference position
M5；
Spindle rotation stop
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G88 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.4.11
Boring Cycle (G89)
Code format:
G89
X_ Y_ Z_ R_ P_ F_ K_
Function: This cycle is used to bore a hole
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
P_ Dwell time at the bottom of a hole;
F_: Cutting feedrate;
K_: Repeated times.
88
Chapter Four
Preparatory Function G Code
G89（G98）
G89（G99）
Initial point
plane
R
P
P
Point R
plane
Z
Z
Fig. 4-4-11-1
This cycle, almost, is absolute indentical with the G85. The different is that this cycle performs a
dwell at the bottom of the hole.
Before specifying G89, use a miscellaneous function (M code) to rotate the spindle.
When the G89 and the M code are specified at a same block, perform the M code at the time of
performing the 1st hole position operation, and then, the system then proceeds the next drilling
operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole only
instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with the program;
perform the above-mentioned M code after executing the current statement.
P is the modal code, the least value of parameter is set by data parameter P281 and the most
value is set by p282. Value P is less than the P281 parameter setting value, which is operated based
upon the least value; if it more than the P282 parameter setting value and it is operated based upon
the most value.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded
a same block with the canned cycle, add or cancel an offset value at the time of positioning to point R;
in the canned cycle modal, if the tool compensation G43, G44 or G49 is placed at one block
separately, the system is then performed the offset value addition or cancellation with real-time.
Axis switching: Cancel the canned cycle before the boring axis can be shifted.
Boring machining: In a block that does not contain X, Y, Z or other miscellaneous axes is not
performed.
Example:
M3 S100；
Spindle rotation
G90 G99 G89 X300 Y-250 Z-150 R-120 P1000 F120； Positioning, bore hole 1, then return to
89
VOLUME I
PROGRAMMING
R
GSK218MC Series Machining CNC System
Programming & Operation Manual
point R then stop that the bottom of the
hole for 1s.
Y-550；
Positioning, bore hole 2, then return to point R
Y-750；
Positioning, bore hole 3, then return to point R
X1000；
Positioning, bore hole 4, then return to point R
Y-550；
Positioning, bore hole 5, then return to point R
G98 Y-750；
Positioning, bore hole 6, then return to initial positon plane
G80；
G28 G91 X0 Y0 Z0 ；
Return to the reference position
M5；
Spindle rotation stop
VOLUME I
PROGRAMMING
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G89 command,
the system then performs the G60 modal.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
4.5
4.5.1
Rigid Cycle G Code
Left-handed Rigid Tapping Cycle G74
Code format:
G74 X_Y_Z_R_P_F_K_
Function: In the rigid method, the working of spindle motor is a servo motor, and this code can be
carried out the left-handed tapping with high speed and high accuracy.
Explanation:
X_Y_: Hole position data
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
P_: The dwell time at the bottom of a hole or the dwell time at the point R.
F_: Cutting feedrate.
K_: Repeated times. (If required)
90
Chapter Four
Preparatory Function G Code
G74（G98）
G74（G99）
Spindle stop
Spindle stop
Motion 1
Motion 2
Spindle
negative
R
Motion 3
Motion 1
Motion 2
Motion 6
Spindle stop
P
Point R plane
Spindle
negative
R
Motion 3
Motion 5
Spindle
positive
Spindle stop
P Motion 4 Z
PMotion 4 Z
Spindle stop
P
Motion 5
Spindle
positive
Fig. 4-5-1-1
Z axis moves to point R at the rapid traverse and performs G74 along with X and Y axes after
positioning, and then spindle reverse. The tapping is performed from point R to Z, when the tapping is
completed, the spindle stops and performs the dwell, then spindle rotates tool retreating from point R
with reverse direction, spindle then stops; consequently, spindle moves to the initial position at a rapid
traverse rate. The feedrate and spindle override are regarded as 100% when tapping is being
performed.
Rigid method: In the position mode (bit 1 of parameter No.:46 is set to 1, K parameter No. :7#7 sets
to 1), to perform M29 S***** before the tapping code can be specified the rigid
method.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded a
same block with the canned cycle, add or cancel an offset value at the time of
positioning to point R; in the canned cycle modal, if the tool compensation G43, G44
or G49 is placed at one block separately, the system is then performed the offset
value addition or cancellation with real-time.
Thread leading: In the feed/min. method, the relationships among the thread leadind, feedrate and
spindle speed as follows:
Feedrate F = screw tap pitch × spindle speed S
For example: Tap a thread hole M12×1.5 on component, the parameter can be
optioned;
S500=500ｒ/min；
F=1.5×500=750mm/min；
Multi-head thread x head numbers = F value
In the feed method per revolution, thread leading equals to feedrate.
91
VOLUME I
PROGRAMMING
Spindle stop
Initial point
plane
GSK218MC Series Machining CNC System
Programming & Operation Manual
For example:
Feed/min.:
Fee/rev.:
Spindle speed 1000r/min；
Spindle speed 1000r/min；
Thread leading 1.0mm；
Thread leading 1.0mm；
Then feedrate of Z axis= 1000*1=1000mm/min; Then feedrate of Z axis=thread leading 1=1mm / r；
G94
Feed/min.
G95
Feed/rev.
G00 X120 Y100；
Positioning
G00 X120 Y100；
Positioning
M29 S1000 ；
Specify a rigid tapping
M29 S1000 ；
Specify a rigid tapping
G74 Z-100 R-20 F1000; Left-handed rigid tapping
G80
G74 Z-100 R-20 F1;Left-handed rigid tapping
Cancel the tapping cycle
VOLUME I
PROGRAMMING
G28 G91 X0 Y0 Z0 Reference position return
M30
G80
Cancel the tapping cycle
G28 G91 X0 Y0 Z0 Reference position return
End-of-program
M30
End-of-program
Restriction:
G code: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of parameter
No.:48 is set to 1)) of group 01 in a same block when using G74 command, the
system then performs the G60 modal.
M code: Spindle is rotated by miscellaneous function M code before specifying G74. If there is no
specified the spindle rotation, the system then adjusts as CW based upon the current
spindle command speed automatically.
When the G74 code and an M code are specified in the same block, the M code is
executed at the time of the first positioning operation. The system then proceeds to
the next drilling operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole
only instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with
the program; perform the above-mentioned M code after executing the current statement.
S command:
If the specified spindle speed exceeds the top spindle speed in tapping (data
parameter P257: the upper limit speed of spindle in tapping cycle), the system then
alarms; the top speed level of the spindle in the rigid tapping is determined by
P94~P296.
F command: If the specified F value exceeds the upper limit value of the cutting feedrate (data
parameter: P96 sets the upper limit value of cutting feed), it is subject to the upper
limit value.
P command: P is the modal code, the least value of parameter is set by data parameter P281 and
the most value is set by p282. Value P is less than the P281 parameter setting value,
which is operated based upon the least value; if it more than the P282 parameter
setting value and it is operated based upon the most value.
Axis shifting: Cancel the canned cycle before shifting the tapping axis. If the tapping axis is changed
92
Chapter Four
Preparatory Function G Code
in rigid tapping mode, the system then shows the No.206 alarm.
Override: The feedrate and spindle rotation feedrate are 100% by default during the rigid tapping; the
machine tool still operates after pressing the feed hold and reset buttons till the
completion of the operation return.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Program restart: The program restart function is disabled in tapping cycle.
Note: When the machining, such as the flexible tapping, rigid tapping or peck tapping, etc. are performed, it is
necessary to firstly cancel the constant surface cutting feed by G97; otherwise, the disorder gear or broken screw tap,
etc. will occur.
Right-handed Rigid Tapping G84
Format:
G84 X_Y_Z_R_P_F_K_
Function: In the rigid method, the control of spindle motor is a servo motor, which can be carried out
the high-speed accuracy tapping. Also, it can be guarantee that the start position of tapping is
consistent in the case of invariable Point R. Namely, the thread still keep order even if
repeated perform the tapping in a position.
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
P_: The dwell time at the bottom of a hole or the dwell time at point R when retracting;
F_: Cutting feedrate;
K_: Repeated times. (If required)
93
VOLUME I
PROGRAMMING
4.5.2
GSK218MC Series Machining CNC System
G84（G98）
G84（G99）
Spindle stop
Spindle stop
Motion 1
Motion 2
Spindle
positive
R
Motion 3
Spindle stop
Programming & Operation Manual
Initial point
plane
Motion 1
Motion 2
Motion 6
Spindle stop
P
Point R plane
Spindle
positive
R
Motion 3
Motion 5
Spindle
negative
Spindle stop
VOLUME I
PROGRAMMING
P Motion 4 Z
Spindle stop
P
Motion 5
Spindle
negative
PMotion 4 Z
Fig. 4-5-2-1
Z axis moves to point R at the rapid traverse and performs G84 along with X and Y axes after
positioning, and then spindle reverse. The tapping is performed from point R to Z, when the tapping is
completed, the spindle stops and performs the dwell, then spindle rotates tool retreating from point R
with reverse direction, spindle then stops; consequently, spindle moves to the initial position at a rapid
traverse rate. The feedrate and spindle override are regarded as 100% when tapping is being
performed.
Rigid method: In the position mode (bit 1 of parameter No.:46 is set to 1, K parameter No. :7#7 sets
to 1), to perform M29 S***** before the tapping code can be specified the rigid
method.
Tool length compensation: When the tool length compensation G43, G44 or G49 is
commanded a same block with the canned cycle, add or cancel an offset value
at the time of positioning to point R; in the canned cycle modal, if the tool
compensation G43, G44 or G49 is placed at one block separately, the system
is then performed the offset value addition or cancellation with real-time.
Screw leading: In the feed/min. mode, the relationships among the screw leading, feedrate and
spindle speed are shown below:
Feedrate F = screw tap pitch × spindle speed S
For example: tap the M12×1.5 screw hole in component, optional parameter;
S500=500ｒ/min；
F=1.5×500=750mm/min；
In multiple thread, the F value can be calculated by multiplying by the numbers of
thread head.
In feed/rev. mode, the thread leading equals to the feedrate.
94
Chapter Four
Preparatory Function G Code
For example:
Feed/min.:
Fee/rev.:
Spindle speed 1000r/min；
Spindle speed 1000r/min；
Thread leading 1.0mm；
Thread leading 1.0mm；
Then feedrate of Z axis= 1000*1=1000mm/min; Then feedrate of Z axis=thread leading 1=1mm / r；
G94
Feed/min.
G95
Feed/rev.
G00 X120 Y100；
Positioning
G00 X120 Y100；
Positioning
M29 S1000 ；
Specify a rigid tapping
M29 S1000 ；
Specify a rigid tapping
G84 Z-100 R-20 F1000; Left-handed rigid tapping
G80
G84 Z-100 R-20 F1;Left-handed rigid tapping
Cancel the tapping cycle
M30
Cancel the tapping cycle
G28 G91 X0 Y0 Z0 Reference position return
End-of-program
M30
End-of-program
Restrictions:
G code: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of parameter
No.:48 is set to 1)) of group 01 in a same block when using G84 command, the
system then performs the G60 modal.
M code: Spindle is rotated by miscellaneous function M code before specifying G84. If there is no
specified the spindle rotation, the system then adjusts as CW based upon the current
spindle command speed automatically.
When the G84 and an M codes are specified in the same block, the M code is
executed at the time of the first positioning operation. The system then proceeds to
the next drilling operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole
only instead fo performing the subsequent holes.
Note: In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed followed with
the program; perform the above-mentioned M code after executing the current statement.
S command:
If the specified spindle speed exceeds the top spindle speed in tapping (data
parameter P257: the upper limit speed of spindle in tapping cycle), the system then
alarms; the top speed level of the spindle in the rigid tapping is determined by
P94~P296.
F command: If the specified F value exceeds the upper limit value of the cutting feedrate (data
parameter: P96 sets the upper limit value), it is subject to the upper limit value.
P command: P is the modal code, the least value of parameter is set by data parameter P281 and
the most value is set by p282. Value P is less than the P281 parameter setting value,
which is operated based upon the least value; if it more than the P282 parameter
setting value and it is operated based upon the most value.
Axis shifting: Cancel the canned cycle before shifting the tapping axis. If the tapping axis is changed
95
VOLUME I
PROGRAMMING
G28 G91 X0 Y0 Z0 Reference position return
G80
GSK218MC Series Machining CNC System
Programming & Operation Manual
in rigid tapping mode, the system then shows the No.206 alarm.
Override: The feedrate and spindle rotation feedrate are 100% by default during the tapping; the
machine tool still operates after pressing the feed hold and reset buttons till the
completion of the operation return.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Program restart: The program restart function is disabled in tapping cycle.
Note: When the machining, such as the flexible tapping, rigid tapping or peck tapping, etc. are performed, it is
necessary to firstly cancel the constant surface cutting feed by G97; otherwise, the disorder gear or broken screw tap,
etc. will occur.
VOLUME I
PROGRAMMING
4.5.3
Peck Tapping (Chip-removal) Cycle
Code format:
G84（or
G74） X_Y_Z_R_P_Q_F_K_
Function: In the peck tapping, cutting is performed for several times until the bottom of the hole.
Explanation:
X_Y_: Hole positioning data;
Z_: Incremental programming means the distance from the specified point R to the bottom of
the hole; absolute programming means the absolute coordinate value at the bottom of the hole;
R_: Incremental programming means the distance from the initial point plane to the point R;
absolute programming means the absolute coordinate value of point R;
P_: The dwell time at the bottom of a hole or at point R when retracting;
Q_: The cutting depth of cutting feed each time;
F_: Cutting feedrate;
V_: Retraction distance d; if it does not specify, which is set by parameter P284.
K_: Repeated times. (If required)
96
Chapter Four
Preparatory Function G Code
G74/G84（G98）
G74/G84（G99）
D=Retraction distance
(High-velocity peck tapping)
D=Retraction distance
(High-velocity peck tapping)
Initial point plane
R
q
Point R
position plane
q
d
q
Point R
position plane
R
d
q
d
q
d
q
Z
Z
G74/G84（G99）
d=Cutting start distance
(Standard peck tapping)
d=Cutting start distance
(Standard peck tapping)
VOLUME I
PROGRAMMING
G74/G84（G98）
Initial point plane
R
q
q
Point R
position plane
q
d
Point R position
plane
R
d
q
d
q
d
q
Z
Z
Fig. 4-5-3-1
Table 4-5-3-1
Peck tapping cycle
Parameter setting
Adoptive tapping method
It is high-speed peck tapping cycle
Peck flexible tapping
cycle
NO:46#1=0 and NO:K007#7=0
when NO:44#5=1.
It is standard peck tapping cycle
when NO:44#5=0.
It is high-speed peck tapping cycle
Peck rigid tapping cycle
NO:46#1=1 and NO:K007#7=1
when NO:44#5=1.
It is standard peck tapping cycle
when NO:44#5=0.
Two peck tapping cycles are available: High-speed peck tapping cycle and standard peck
tapping cycle, which are determined by bit 1 of parameter No.: 46.
Peck flexible tapping cycle:
97
GSK218MC Series Machining CNC System
Programming & Operation Manual
When bit 1 of parameter No.: 46 equals to 0 and bit 7 of parameter No.: K007
equals to 0, which are the flexible peck tapping cycle. In the peck flexible tapping
method, the high-speed peck tapping cycle and standard peck flexible tapping
cycle are available, which can be set by bit 5 of parameter No.: 44 .
High-speed peck tapping cycle:
It is the high-speed peck tapping cycle when bit 5 of parameter No.: 44 sets to 1:
rapid traverse to point R after positioning along with the X and Y axes. From point
R, cutting is performed with depth Q (depth of cut for each cutting feed) , then the
tool is retracted by distance d (It is specified by canned parameter V, if it does not
specify, it then sets by data parameter P284), which is set the rigid tapping
tool-retraction by the bit 4 of parameter No.: 44, the override is enabled, is specified
VOLUME I
PROGRAMMING
retraction speed override by bit 3 of parameter No.: 45, is set the rigid tapping
in-feed, tool-retraction whether using the same time constant by bit 2 of parameter
No.: 45, is set whether the feedrate selection and override cancellantion signal are
enabled in the rigid tapping by bit 4 of No.: 45. When point Z has been reached, the
spindle is stopped, then rotated in the reverse direction for retration.
Standard peck (flexible) tapping cycle:
It is the standard peck tapping cycle when bit 5 of parameter No.: 44 sets to 0:
rapid traverse to point R after positioning along with the X and Y axes. From point
R, cutting is performed with depth Q (depth of cut for each cutting feed), and then
return to point R; whether the overrider in rigid tapping is enabled which is set by bit
4 of parameter No.44; specify the retraction feedrate by bit 3 of parameter No.:45;
the distance d (it is set by data parameter P284) from the point R to the end of
cutting, then perform the cutting again based upon the value of the cutting feedrate
F; whether using the same time constant in the in-feed, tool-retraction, which is set
by bit 2 of parametr No.45. When point Z has been reached, the spindle is stopped,
then rotated in the reverse direction for retration.
Standard peck (rigid) tapping cycle:
In the position mode (bit 1 of parameter No.:46 is set to 1, K parameter No. :7#7
sets to 1), specify M29 S***** as the peck rigid tapping cycle before the tapping
code; here, use the standard peck tapping cycle method, and its setting method is
indentical with the flexible standard peck tapping one.
Tool length compensation: When the tool length compensation G43, G44 or G49 is commanded a
same block with the canned cycle, add or cancel an offset value at the time of
positioning to point R; in the canned cycle modal, if the tool compensation G43,
G44 or G49 is placed at one block separately, the system is then performed the
offset value addition or cancellation with real-time.
Restrictions:
98
Chapter Four
Preparatory Function G Code
G code: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of parameter
No.:48 is set to 1)) of group 01 in a same block when using G74/G84 command, the
system then performs the G60 modal.
M code:
Use the miscellaneous function M code to rotat the spindle before specifying the G74/G84.
if the spindle rotation does not perform, the system is then automatically rotated
based upon the current spindle in R plane, and then adjust to the CCW.
When the G74/G84 and an M codes are specified in the same block, the M code is
executed at the time of the first positioning operation. The system then proceeds to
the next drilling operation.
When K is used to specify the repeated times, the M code is executed for the 1st hole
only instead fo performing the subsequent holes.
followed with the program; perform the above-mentioned M code after executing the
current statement.)
S command:
If the specified spindle speed exceeds the top spindle speed in tapping (data
parameter P257: the upper limit speed of spindle in tapping cycle), the system then
alarms; the top speed level of the spindle in the rigid tapping is determined by
P94~P296.
F command: If the specified F value exceeds the upper limit value of the cutting feedrate (data
parameter: P96 sets the upper limit value), it is subject to the upper limit value.
P command: P is the modal code, the least value of parameter is set by data parameter P281 and
the most value is set by p282. Value P is less than the P281 parameter setting value,
which is operated based upon the least value; if it more than the P282 parameter
setting value and it is operated based upon the most value.
Axis shifting: Cancel the canned cycle before shifting the tapping axis. If the tapping axis is changed
in rigid tapping mode, the system then shows the No.206 alarm.
Override: The feedrate and spindle rotation feedrate are 100% by default during the tapping; the
machine tool still operates after pressing the feed hold and reset buttons till the
completion of the operation return.
Cutter compensation: In this canned cycle command, cutter compensation is ignored due to the
command function is regardless of the cutter compensation.
Program restart: The program restart function is disabled in tapping cycle.
Note: When the machining, such as the flexible tapping, rigid tapping or peck tapping, etc. are performed, it is
necessary to firstly cancel the constant surface cutting feed by G97; otherwise, the disorder gear or broken screw tap,
etc. will occur.
99
VOLUME I
PROGRAMMING
(In the current version, M00, M01, M02, M06, M30, M98 and M99 are performed
GSK218MC Series Machining CNC System
4.6
Programming & Operation Manual
Compound Cycle G Code
Compound comparison table (G22～G38)
Table 4-6-1
G code
Drilling
Operation at the
Tool-retraction
(-Z direction)
bottom of a hole
operation
Purpose
(-Z direction)
G22
VOLUME I
PROGRAMMING
G23
G24
G25
Cutting feed
Rapid traverse
Groove rough-milling of inner
circle along CCW
Cutting feed
Rapid traverse
Groove rough-milling of inner
circle along CW
Cutting feed
Rapid traverse
Fine-milling cycle of full circle
along CCW
Cutting feed
Rapid traverse
Fine-milling cycle of full circle
along CW
G26
G32
G33
G34
G35
G36
G37
G38
Cutting feed
Rapid traverse
Excircle fine-milling cycle
along CCW
Cutting feed
Rapid traverse
Excircle fine-milling cycle
along CW
Cutting feed
Rapid traverse
Rectangluar groove
rough-milling along CCW
Cutting feed
Rapid traverse
Rectangluar
rough-milling along CW
Cutting feed
Rapid traverse
Fine-milling cycle of the inner
rectangular groove along CCW
Cutting feed
Rapid traverse
Fine-milling cycle of the inner
rectangular groove along CW
Cutting feed
Rapid traverse
Fine-milling cycle
ex-rectangular CCW
Cutting feed
Rapid traverse
Fine-milling cycle
ex-rectangular CW
Restriction:
The tool radius offset (D) will be ignored during the canned cycle position.
100
groove
Chapter Four
4.6.1
Preparatory Function G Code
Groove Rough-Milling of Inner Circle (G22/G23)
Code format:
G22
G98/G99
X_
Y_
Z_
R_
I_
L_
W_
Q_
V_
D_
F_
K_
G23
Function: The multiple circular arc interpolation can be performed by helical method from the
beginning of the center till the round groove is machined by the program dimension.
Explanations:
G22: Groove rough-milling of inner circle along CCW;
G23: Groove rough-milling of inner circle along CW;
Z: Machining depth, its an absolute position in G90; it is a position related to the R reference
surface in G91;
R: R reference surface position, it is absolute position in G90, the start position related to this
block in G91;
I: Incircle groove radius;
L: The width increment by cutting within XY plane.
W: Cutting depth along with the Z axis at the 1st time, it is downward from R reference surface,
which should be more than 0 (If the cutting depth is more than the position at the bottom of
the groove, then it is machined directly based upon the groove position);
Q: Cutting depth of each cutting feed;
V: The distance from the unprocessed surface during cutting at the rapid traverse rate;
D: Tool compensation number, take out the corresponding tool compensation value based upon
the provided series number;
K_: Repeated times.
Cycle processes:
(1) Rapid positioning to the specified point (X, Y), offset a tool radius D along with the X axis
negative direction, and then multiple the cutting coefficient position of the helix;
(2) Move to point R plane at the rapid traverse rate;
(3) Downward the cutting W distance depth with helical method at the rapid traverse rate →
feed to the circle center
(4) The circle surface with radius I is milled with helix step by step by L value for each time
where from center to outside;
(5) Z axis returns to R reference surface at the rapid traverse rate;
(6) Rapid positioning to the start position along with the X and Y axes;
(7) Z axis descends to the distance from the unproceeded surface V at the rapid traverse
rate;
(8) Cutting (Q+V) depth downward along Z axis;
101
VOLUME I
PROGRAMMING
X, Y: The start position of X, Y plane;
GSK218MC Series Machining CNC System
Programming & Operation Manual
(9) Repeat the operations from (4) to (8) till to the total cutting depth on the surface is
machined;
(10) Return to initial point plane or point R plane based upon the different specifications of
G98 or G99.
Code path:
(1)
Initial point
(2)
(6)
R
Rapid feed
VOLUME I
PROGRAMMING
Cutting feed
(3)
(7)
(5)
(8)
(4)
Fig. 4-6-1-1
Fig. 4-6-1-2
Notice:
1. It is surposed to change the bit 1 of parameter No.12 into 1 when using this code.
2. The coefficient setting of helical cutting radius in the groove cycle should be more than 0, which is set by data
parameter P269.
For example: An inner-circle groove is performed by rough-milling by canned cycle G22 code, refer
to the following figure:
102
Chapter Four
Preparatory Function G Code
Y
Z
Start point
position Z=50
50
Start
Point R plane position
Z=5
5
0
X
L=10
X
-50
-53
I=50
Fig. 4-6-1-3
VOLUME I
PROGRAMMING
G90 G00 X50 Y50 Z50； （G00 rapid positioning）
G99 G22 X25 Y25 Z-50 R5 I50 L10 W20 Q10 V10 D1 F800； (Incircle groove
rough-millingcycle is performed)
G80 X50 Y50 Z50；
(Cancel the canned cycle, then return from point R plane)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G22/G23
command, the system then performs the G60 modal.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
4.6.2
Fine-milling Cycle of the Full Incircle (G24/G25)
Code format:
G24
G98/G99
X_
Y_
Z_
R_
I_
J_
D_
F_
K_
G25
Function: Tool performs a whole circle with fine-milling inside the circle based upon the specified
radius value I and the direction, and then return after fine-milling is executed.
Explanations:
G24: Fine-milling cycle inside the whole circle along CCW.
G25: Fine-milling cycle inside the whole circle along CW.
X, Y: The start position of the X, Y plane;
Z: Machining depth, it is absolute position in G90; it is a position related to the R reference
surface in G91;
R: R reference surface position, it is the absolute position in G90; it is a position related to the
103
GSK218MC Series Machining CNC System
Programming & Operation Manual
start of this block in G91;
I: Fine-milling circle radius;
J: The distance between the fine-milling start and the center of the fine-milling;
D: Tool compensation number, take out the corresponding tool compensation value based
upon the provided series number;
K_: Repeated times.
Cycle processes:
(1) Rapid positioning to the postion along with XY plane;
(2) Descend to point R plane at the rapid traverse rate;
(3) Cutting feed to the start of the bottom of a hole;
(4) The transition arc 1 is regarded as path to perform an arc interpolation from the start;
VOLUME I
PROGRAMMING
(5) The fine-milling incircle is treated as a path to perform the whole-circle interpolation;
(6) The transition arc 4 is regarded as a ptht to perform the arc interpolation and then return
to the start;
(7) Return to initial point plane or point R plane based upon the different specifications of G98
or G99.
Code path:
4: Fine-milling cycle inside the whole circle CCW
Y
G25: Fine-milling cycle inside the whole circle CW
Y
2I
2I
3
2
J
J
4
Center Starting
point
3
Tool
Cutter
center path
1
1
X
Center Starting
point
2
Incicle
boundary
Cutter center
path
Tool
4
X
Incircle
boundary
Fig. 4-6-2-1
Notice: It is suggested to change the bit 1 of parameter No.12 into 1 when using this code.
For example: The fine-milling is performed for the roughed circle groove by canned cycle G24 code;
refer to the following figure.
104
Chapter Four
Preparatory Function G Code
Y
Z
I=50
Start position
Z=50
50
2
Point R plane
position Z=5
5
0
J=10
4
X
1
Center Start
3
（X25,Y25）
X
-50
-53
Cutter center
path
Incircle
boundary
VOLUME I
PROGRAMMING
Fig. 4-6-2-2
G90 G00 X50 Y50 Z50；
(G00 rapid positioning)
G99 G24 X25 Y25 Z-50 R5 I50 J10 D1 F800；(Canned cycle start, perform the incircle
fine-milling cycle at the bottom of the hole)
G80 X50 Y50 Z50；
(Cancel the canned cycle, return to the point R plane)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G24/G25
command; otherwise, G24/G25 will be replaced by the G code of group 01.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
4.6.3
Excircle Fine-milling Cycle (G26/G32)
Code format:
G26
G98/G99
X_
Y_
Z_
R_
I_
J_
D_
F_
K_；
G32
Function: Tool performs a whole circle at the excircle with fine-milling based upon the specified
radius value and its direction, and then return.
Explanations:
G26: Excircle fine-milling cycle CCW
G32: Excircle fine-milling cycle CW
X, Y: The start position of X, Y plane;
Z: Machining depth, it is absolute position in G90; it is the position related to the R reference
105
GSK218MC Series Machining CNC System
Programming & Operation Manual
surface in G91;
R: R reference surface position, it is the absolute position in G90; it is the position related to
the start of this block in G91;
I: Fine-milling circle radius;
J: The distance between the fine-milling start and the circle edge;
D: Tool compensation number, take out the corresponding tool compensation value based
upon the offered series number;
K: Repeated times. (If required)。
Cycle processes:
(1) Positioning to the XY plane at the rapid traverse rate;
(2) Descend to point R plane at the rapid traverse rate;
VOLUME I
PROGRAMMING
(3) Cutting feed to the bottom of a hole;
(4) The transition arc 1 is regarded as path to perform arc interpolation from the start;
(5) Perform the whole circle interpolation based upon the path of the arc 2 and 3;
(6) The transition arc 4 is regarded as path to perform the arc interpolation and then return to
the start;
(7) Return to initial point plane or point R plane based upon the different specifications of G98
or G99
Code path:
G32: Excircle fine-milling cycle CW
Y
2I+D
3
G26: Excircle fine-milling cycle CCW
Y
2I+D
2
1
4
Center
Excircle
boundary
J
1
X
Start
point
Tool
3
Cutter center path
4
Center
J
Excircle
boundar
Tool
y
2
Cutter center path
X
Start
point
Fig. 4-6-3-1
Explanation:
The interpolaton both the transition arc and the fine-milling arc are inconsistent when the
finish-milling is perfirmed at the excircle; the interpolation direction in the code explanation is the
interpolation direction of the fininsh-milling arc.
For example: The fine-milling is performed for the roughed circle groove by canned cycle G26 code;
refer to the following figure.
106
Chapter Four
Preparatory Function G Code
Y
2
Z
Start position
Z=50
50
Point R plane
position Z=5
5
0
4
I=50
Center
Excircle
boundary
1
J=30
(X25,Y25）
Start
Tool
3
X
-50
-53
X
Cutter center path
Fig. 4-6-3-2
G90 G00 X50 Y50 Z50；
(G00 rapid positioning)
G99 G26 X25 Y25 Z-50 R5 I50 J30 D1 F800； (Canned cycle start, Excircle fine-milling cycle
G80 X50 Y50 Z50；
(Cancel the canned cycle, return from the point R plane)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G26/G32
command, the system then executes G60 modal.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
4.6.4
Rectangular Groove Rough-milling (G33/G34)
Code format:
G33
G98/G99
X_
Y_
Z_
R_
I_
J_
L_
W_
Q_
V_
U_
D_
F_
K_
G34
Function: Start from the center of the rectangle, the specified parameter data is regarded as the
linear cutting cycle till the rectangular groove is machinied based upon the programmed dimension.
Explanations:
G33: Rectangular groove rough-milling CCW;
G34: Rectangular groove rough-milling CW;
X, Y: The start position on the X,Y plane;
Z: Machining depth, it is the absolute position in G90; it is the positon related to the R
reference surface in G91;
R: R reference surface position, it is the absolute position in G90; it is the position related to
the start in this block in G91;
I: The width of the rectangular groove along X axis direction;
107
VOLUME I
PROGRAMMING
performs at the bottom of a hole)
GSK218MC Series Machining CNC System
Programming & Operation Manual
J: The width of the rectangular groove along Y axis direction;
L: The cutting width increment within the specified plane;
W: Cutting along the Z axis at the 1st time is the downward distance from the R reference
surface, which should be more than 0 (If the cutting depth for the 1st time exceeds the
position at the bottom of the groove, it will be directly machined based upon the position of
groove bottom);
Q: Cutting depth of each cutting feedrate;
V: The distance from the unprocessed surface during the cutting at the rapid traverse rate;
U: Corner arc radius; without corner arc transition if it omits;
D: Tool compensation number, take out the corresponding tool compensation value based
upon the offered series number;
K_: Repeated times.
(1) Positioning to the helical cutting start position along XY plane at the rapid traverse rate;
(2) Descend to the point R plane at the rapid traverse rate;
(3) Helical cutting W distance based upon that the radius compensation value miltiples the
value of data parameter No.269 is regarded as the diameter;
(4) Feed to the rectangular center position;
(5) The rectangular surface milled increasing by L value for each time where from center to
outside;
(6) Z axis returns to R refernce surface at the rapid traverse rate;
(7) Positioning to helix cutting start position along the XY plane at the rapid traverse rate;
(8) Z axis descends to the distance from the unprocessed plane V;
(9) The cutting (Q+V) depth downward along Z axis;
(10) Repeat the operations from (4) to (9) till to the total cutting depth on the surface is
machined;
(11) Return to initial point plane or point R plane based upon the different specifications of
G98 or G99.
Code path:
G33 rectangular groove rough-milling CCW
G34 rectangular groove rough-milling CW
Note: λ is the coefficient of
helical cutting radius.
U
Cutter center path
L
U U-R
（U-R）/2
L
Cutter center
path
U-R
（U-R）/2
6
In-feed
point
4
1
5 7
6
2
D*
Tool
Rectangular
groove boundary
I
7
4
3
D*
5
Tool
I
Fig. 4-6-4-1
108
In-feed
point
1
J
2
3
J
VOLUME I
PROGRAMMING
Cycle processes:
Rectangular
groove boundary
Chapter Four
Preparatory Function G Code
Notice: It is suggested to change the bit 1 of parameter No.12 into 1 when using this code.
For example: The rough-milling is performed within a rectangle groove by canned cycle G33 code;
refer to the following figure:
Z
Y
U=5
L=10
Start position
Z=50
50
J=50
Point R plane
position Z=5
5
0
Tool
X
-50
-53
X
I=70
G90 G00 X50 Y50 Z50；
（G00 rapid positioning）
G99 G33 X25 Y25 Z-50 R5 I70 J50 L10 W20 Q10 V10 U5 D1 F800； (Perform the groove
rough-milling cycle within rectangle)
G80 X50 Y50 Z50；
(Cancel the canned cycle, return from the point R plane)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G33/G34
command; otherwise, G33/G34 will be replaced by the G code of group 01.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
4.6.5
Fine-milling Cycle within Rectangular Groove (G35/G36)
Code format:
G35
G98/G99
X_
Y_
Z_
R_
I_
J_
L_
U_
D_
F_
K_；
G36
Function: Tool is performed the fine-milling with the specified width and direction, and then return
after the fine-milling is completed.
Explanations:
G35: Fine-milling cycle inside the rectangular groove CCW.
G36: Fine-milling cycle inside the rectangular groove CW.
X, Y: The start position on X, Y plane;
Z: Machining depth, it is the absolute position inG90; it is the position related to the R
reference surface in G91;
109
VOLUME I
PROGRAMMING
Fig. 4-6-4-2
GSK218MC Series Machining CNC System
Programming & Operation Manual
R: R reference surface position, it is the absolute position in G90; it is the position related to
the start of this block in G91;
I: The width along with rectangular X axis direction;
J: The width along with rectangular Y axis direction;
L: The distance from the fine-milling start to the rectangular edge positive direction along X
axis;
U: Corner arc radius; there is no corner arc transition if it omits. When 0＜｜U｜＜tool radius,
the alarm then occurs;
D; Cutter compensation number, take out the corresponding cutter compensation value based
upon the provided series number;
K: Repeated times.
(1) Positioning to the start position on XY plane at the rapid traverse rate;
(2) Descend to the point R plane at the rapid traverse rate;
(3) Cutting feed to the bottom of a hole;
(4) Perform the arc interpolation from the start based upon that the transition arc 1 is
regarded as the path;
(5) Perform the linear and arc interpolation based that the 2-3-4-5-6 are treated as path;
(7) Return to start to perform the arc interpolation based upon that the transition arc 7 is
regarded as path;
(7) Return to initial point plane or point R plane based upon the different specifications of G98
or G99.
Code path:
G35 rectangular groove fine-milling cycle CCW
G36 rectangular groove fine-milling cycle CW
L
U
L
3
Tool
Cutter center
path
U
5
Tool
Cutter center
path
2
6
7
Start
4
1
6
1
Rectangular
groove boundary
J
4
J
VOLUME I
PROGRAMMING
Cycle processes:
Start
7
2
5
3
I
I
Rectangular
groove boundary
Fig. 4-6-5-1
Notice: It is suggested to change the bit 1 of parameter No.12 into 1 when using this code.
For example: The fine-milling is performed for the roughed groove by canned cycle G35 code; refer
to the following figure.
110
Chapter Four
Preparatory Function G Code
Y
L=30
5
0
Start position
Z=50
Tool
3
2
Point R plane
position Z=5
7
4
Start
（X10,Y0）
1
X
6
5
X
-50
-53
J=50
50
U=10
Z
I=80
Fig. 4-6-5-2
G90 G00 X50 Y50 Z50；
(G00 rapid positioning)
G99 G35 X10 Y0 Z-50 R5 I80 J50 L30 U10 D1 F800； (Perform the rectangular groove inner
canned cycle method)
G80 X50 Y50 Z50；
(Cancel the canned cycle, return to the point R plane)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G35/G36
command, the system then executes G60 modal.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
4.6.6
Fine-milling ccle Outside the Rectangle (G37/G38)
Code format:
G37
G98/G99
X_
Y_
Z_
R_
I_
J_
L_
U_
D_
F_
K_
G38
Function: Tool is performed the fine-milling with the specified width and direction, and then return
after the fine-milling is completed.
Explanations:
G37: Fine-milling cycle outside the rectangular groove CCW.
G38: Fine-milling cycle outside the rectangular groove CW.
X, Y: The start position on X, Y plane;
Z: Machining depth, it is the absolute position inG90; it is the position related to the R
reference surface in G91;
R: R reference surface position, it is the absolute position in G90; it is the position related to
111
VOLUME I
PROGRAMMING
milling to the bottom of a hole in the
GSK218MC Series Machining CNC System
Programming & Operation Manual
the start of this block in G91;
I: The width along with rectangular X axis direction;
J: The width along with rectangular Y axis direction;
L: The distance from the fine-milling start to the rectangular edge positive direction along X
axis;
U: Corner arc radius; there is no corner arc transition if it omits;
D; Cutter compensation number, take out the corresponding cutter compensation value based
upon the provided series number;
K: Repeated times.
Cycle processes:
(1) Positioning to the start position on XY plane at the rapid traverse rate;
VOLUME I
PROGRAMMING
(2) Descend to the point R plane at the rapid traverse rate;
(3) Cutting feed to the bottom of a hole;
(4) Perform the arc interpolation from the start based upon that the transition arc 1 is
regarded as the path;
(5) Perform the linear and arc interpolation based that the 2-3-4-5-6 are treated as path;
(7) Return to start to perform the arc interpolation based upon that the transition arc 7 is
regarded as path;
(8) Return to initial point plane or point R plane based upon the different specifications of G98
or G99.
Code path:
G37 Fine-milling cycle
outside the rectangle CCW
G38 Fine-milling cycle
outside the rectangle CW
L
L
7
6
1
4
J
4
5
1
7
6
5
I
Tool
Cutter
center path
J
2
Cutter
center path
U
U
3
Rectangular
groove boundary
2
3
I
Tool
Rectangular
groove boundary
Fig. 4-6-6-1
Explanation:
The transition arc is inconsistent with the interpolation direction of the fine-milling arc when the
finish-milling is performed outside the rectangle. The interpolation direction in the code explanation is
the one of the fine-milling arc.
For example: Fine-milling outside the rectangle is performed by canned cycle G37 code.
G90 G00 X50 Y50 Z50； (G00 rapid positioning)
G99 G37 X25 Y25 Z-50 R5 I80 J50 L30 U10 D1 F800；(Perform the fine-milling outside the
112
Chapter Four
Preparatory Function G Code
rectangle at the bottom of a hole by
canned cycle)
G80 X50 Y50 Z50；
(Canecl the canned cycle, return from the point R)
M30；
Restriction: Fail to specify the G code (From G00 to G03, G60 are the modal codes (bit 0 of
parameter No.:48 is set to 1)) of group 01 in a same block when using G37/G38
command, the system then executes G60 modal.
Cutter compensation: In this canned cycle command positioning, tool radius offset is ignored; call
the specified cutter compensation by program in the procedure of in-feed.
VOLUME I
PROGRAMMING
4.6.7 Canned Cycle Cancel (G80)
Code format: G80
Function: Canned cycle canel
Explanation:
Cancel the overall canned cycles, and then perform the normal operation, at the same time, the
point R and Z are cancelled, as well the other drilling, boring data are eliminated, too.
Example:
M3 S100；
Spindle rotation
G90 G99 G88 X300 Y-250 Z-150 R-120 F120；
Positioning, bore hole 1, then return to the point R
Y-550；
Positioning, bore hole 2, then return to the point R
Y-750；
Positioning, bore hole 3, then return to the point R
X1000；
Positioning, bore hole 4, then return to the point R
Y-550；
Positioning, bore hole 5, then return to the point R
G98 Y-750；
Positioning, bore hole 1, then return to the initial position plane
G80；
G28 G91 X0 Y0 Z0；
M5；
Return to the reference position and then cancel the canned cycle.
Spindle rotation stop
M30；
For example:
The following figure uses the tool length compensation, which are expressed the usage of the
canned cycle totally.
113
GSK218MC Series Machining CNC System
Programming & Operation Manual
350
Reference position
100
#7
#2
#8
100
#5
#12
#3
Unit: mm
#6
#10
200
100
Y
#11
200
100
#1
#9
#4
#13
X
400
150
250
250
150
VOLUME I
PROGRAMMING
# 1～ 6... drill Φ10 hole
# 7～10...drill Φ20 hole
#11～13..bore Φ95 hole
Position return
250
Start position
Z
50
50
Unit:mm
X
30
20
T15
T31
150
190
200
T11
Fig. 4-6-7-1
The value of offset No.11 is 200, No.15 is 190 and No.31 is 150, which are separately set as the
offset. The program are shown below:
114
N001 G92 X0 Y0 Z0 ；
Coordinate system set at the reference point
N002 G90 G00 Z250 T11 M6 ；
Tool-change
N003 G43 Z0 H11 ；
Plane tool length compensation is performed
Chapter Four
Preparatory Function G Code
at the initial point
N004 S300 M3 ；
N005 G99 G81 X400 Y-350 ；
Z-153 R-97 F120 ；
N006 Y-550 ；
N007 G98 Y-750 ；
N008 G99 X1200 ；
N010 G98 Y-350 ；
N011 G00 X0 Y0 M5 ；
N012 G49 Z250 T15 M6 ；
Machine #1 hole after positioning.
Machine #2 hole after positioning, then return
to point R plane.
Machine #3 hole after positioning, then return
to point initial point plane.
Machine #4 hole after positioning, then return
to point R plane.
Machine #5 hole after positioning, then return
to point R plane.
Machine #6 hole after positioning, then return
to point initial point plane.
Return to reference position, spindle then
stops
Cancel the tool length compensation, then
tool-change performs.
N013 G43 Z0 H15 ；
Initial point plane, tool length compensation
N014 S200 M3 ；
Spindle start.
N015 G99 G82 X550 Y-450 ；
Machine #7 hole after positioning, then return
Z-130 R-97 P30 F70 ；
to point R plane.
N016 G98 Y-650 ；
N017 G99 X1050 ；
N018 G98 Y-450 ；
N019 G00 X0 Y0 M5 ；
N020 G49 Z250 T31 M6 ；
VOLUME I
PROGRAMMING
N009 Y-550 ；
Spindle start.
Machine #8 hole after positioning, then return
to point initial point plane.
Machine #9 hole after positioning, then return
to point R plane.
Machine #10 hole after positioning, then
return to point initial point plane.
Return to reference point, spindle stops.
Cancel the tool length compensation, then
prform the tool-change.
N021 G43 Z0 H31 ；
Initial point plane tool length compensation.
N022 S100 M3 ；
Spindle start.
N023 G85 G99 X800 Y-350 ；
Machine #11 hole after positioning, then
Z-153 R47 F50 ；
return to point R plane.
N024 G91 Y-200 ；
Machine #12, #13 holes after positioning, then
Y-200 ；
return to point R plane.
115
GSK218MC Series Machining CNC System
Programming & Operation Manual
N025 G00 G90 X0 Y0 M5 ；
Return to reference point, then spindle stops
N026 G49 Z0 ；
Cancel the tool length compensation
N027 M30 ；
Program stops
4.7
Tool Compensation G Code
4.7.1
Tool Length Compensation G43, G44 and G49
Function:
G43 specifies the positive compensation of tool length.
VOLUME I
PROGRAMMING
G44 specifies the negative compensation of tool length.
G49 cancels tool length compensation.
Format:
System supports A/B tool length offset methods, which can be set by bit 0 of parameter No.:39.
Method A:
G43
G44
Z_ H_ ；
Method B:
G17 G43 Z_H；
G17 G44 Z_H；
G18 G43 Y_H；
G18 G44 Y_H；
G19 G43 X_H；
G19 G44 X_H；
Tool length offset method cancel: G49 or H0.
Explanation:
The purose of the above-mentioned codes is specified a end position of the specified axis and
then moves an offset. The D-value of imaged tool length value in programming and the tool length
value used in the actual machining are set in the offset register in advance; and therefore, the
component machining can be performed by the tool with different length based upon changing the
tool length compensation value, instead of altering the program.
G43 and G44 are specified different offset direction; and the offset number can be specified by
H code.
1. Offset direction
G43: Positive offset (It is the most common offset method)
G44: Negative offset
116
Chapter Four
Preparatory Function G Code
The specified axis in the program moving with the command end coordinate value addes the
offset value (It is set at the offset register) specified by H code regardless of the absolute value code
or incremental value code. In G44, deduct the offset value specified in H code, and then its coordinate
value calculated is regarded as the end coordinate value.
G43 and G44 are modal G codes, which are enabled before encountering other G codes in the
same group.
2. The specification of offset value
The offset length offset number is specified by H code, the corresponding offset value of the
offset number adds or subtracts to the code value moving with Z axis in program, and then becomes
the new Z axis movement code. H00～H255 can be specified according to the offset numbers.
The setting range of the offset values are shown below:
VOLUME I
PROGRAMMING
Table 4-7-1-1
Range
Compensation value H (input by mm)
-999.999 mm～+999.999mm
Compensation value H (input by inch)
-39.3700 inch～+39.3700 inch
Offset No.00 means that H00 is corresponding with the offset value 0, which can not be set in
system.
Notice: When the offset value is changed due to the offset number, only the new offset value
replaces the old one instead of adding. For example:
H01......................... ................offset value 20
H02.......................... ............... offset value 30
G90 G43 Z100 H01 ； ......... Z moves to 120
G90 G43 Z100 H02 ； ......... Z moves to 130
3. The effective sequence of offset number
The current offset number will be immediately enabled once the length offset modal is set up.
However, the new offset value will immediately replace the old one if the offset number is changed.
O×××××；
G43 Z10 H01； (1) Offset number H01 is enabled
G44 Z20 H02； (2) Offset number H02 is enabled
Z30 H03；
(3) Offset number H03 is enabled
G49；
(4) Cancel the tool offset at the end of this block
M30；
4. Cancel the tool length compensation
117
GSK218MC Series Machining CNC System
Programming & Operation Manual
Cancel the tool compensation by G49 or H00. The system will immediately cancel the tool length
compensation after G49 is specified. The compensation axis address and compensation should be
compiled followed with the H00; otherwise, the tool length compensation can not be cancelled.
Notice: 1. The method B of tool length offset is performed after along more than two axes, cancel the offset of
overall axes by G49, and the offset value of axis vertical to the specified plane is only cancelled by
H00.
2. It is suggested that the establishment and cancellation of length compensation adds to the movement code
along Z axis; otherwise, the establishment and length compensation cancellation will be performed at the
current point; and therefore, it is better to confirm that the Z axis is on the safety height when using G49,
prevent the the workpiece from impacting or damaging.
5. The concrete example of tool length compensation
VOLUME I
PROGRAMMING
(A)
Tool length compensation (Machining hole #1, #2 and #3)
(B)
H01= offset value -4
Y
#1
20
X
#3
⑥
30
Unit: mm
⑨
①
30
#2
13
50
30
120
Actual position
Compensation
value (E=4mm)
Programming position
②
③
⑤
⑦
④
⑧
Fig. 4-7-1-1
N1 G91 G00 X120 Y80 ；..……
⑴
N2 G43 Z-32 H01 ；...........……… ⑵
N3 G01 Z-21 F200 ；................... …⑶
N4 G04 P2000 ；........................ . ⑷
N5 G00 Z21 ；....................... ......….⑸
N6 X30 Y-50 ；............... .............….⑹
118
⑩
12
11
8
Unit: mm
22
X
30
18
3
35
Z
Chapter Four
Preparatory Function G Code
N7 G01 Z-41 F200 ；............ ......…..⑺
N8 G00 Z41 ；....................... ......…..⑻
N9 X50 Y30 ；........................ …... ⑼
N10 G01 Z-25 F100 ；............ .....….⑽
N11 G04 P2000 ；...................... ...…⑾
N12 G00 Z57 H00 ；................. ... ....⑿
N13 X-200 Y-60 ；.............. ... . .........⒀
N14 M30 ；
Cutter Compensation G40/G41/G42
VOLUME I
PROGRAMMING
4.7.2
Code format:
G41 D_ X_Y_；
G42 D_ X_Y_；
G40
X_Y_；
Function:
G41 specifies the left compensation of tool movement direction.
G42 specifies the right compensation of tool movement direction.
G40 Cutter compensation cancellation.
Explanations:
1. Cutter compensation function
The following figure shows that the tool with radius R cuts the workpiece A, tool center path
is shown as B in the figure; the distance from path B to A is R. The distance of tool offset
workpiece A radius is called compensation.
B (Tool center path compensation
A (Programming path)
R
Vector
Compensation and vector
Fig. 4-7-2-1
Porgrammer uses the cutter compensation mode to compile the machining program, during
machining, measure the tool diameter and record the register of CNC, and then the tool path
119
GSK218MC Series Machining CNC System
Programming & Operation Manual
becomes the compensation path B.
2. Compensation value (D value)
The radius offset number is specified by D code, which is the cooresponding offset value is
added or deducted to the movement code value in program, so that the new movement code
forms. The offset numbers can be specified D00～D255 based upon the requirements. Whether
the radius compensation value is set by diameter or radius by bit 7 of parameter No.: 40.
The compensation value corresponding offset can be set the offset register in advance by
using LCD/MDI panel.
The setting range of compensation value is shown below:
Table 4-7-2-1
VOLUME I
PROGRAMMING
Range
Compensation value D (mm)
-999.999ｍｍ～+999.999ｍｍ
Compensation D (inch)
-39.3700 inch～+39.3700 inch
Notice: The system regards the compensation value of D00 is 0 by default, user can neither set nor
modify.
The compensation plane should be performed after cancelling the compensation mode. The
system will alarm if the compensation plane changes without cancelling compensation mode.
3. Plane selection and vector
The compensation calculation is performed within the plane selected by G17, G18 and G19.
This plane is called compensation plane. For example, when the XY plane is selected, the
compensation and vector calculations can be executed by (X, Y) in program. The coordinate
value of the axis without the compensation plane is regardless of the compensation.
Simultaneously, 3 axes are controlled, only the tool path shadowed on the compensaton
plane is compensated.
The alteration of compensation plane should be performed after cancelling the
compensation mode.
Table 4-7-2-2
Code
Plane compensation
G17
X – Y plane
G18
Z - X plane
G19
Y - Z plane
4. G40, G41 and G42
The cancellation and performance of cutter compensation is commanded by G40, G41 and
G42 of which they are defined a modal to affirm the value or the direction of compensation vector
combined with the G00 or G01 and codes.
120
Chapter Four
Preparatory Function G Code
Table 4-7-2-3
G code
Function
G40
Cutter compensation cancellation
G41
Left-compensation of tool radius
G42
Right-compensation of tool radius
5. G53, G28 and G30 codes in cutter compensation method
When specifying G53, G28 or G30 code in cutter compensation mode, the offset vector of
tool radius offset axis is cancelled (Wherein, it is cancelled when G53 moves to the specified
position and when G28, G30 moves to the reference position.) when moving to the specified
same block with the G41//G42, the radius compensation is cancelled when the overall axes are
moved to the command position. When G28 or G30 is shared a block with G41//G42, the overall
axes are cancelled the radius compensation when moving to the reference position. The vector
cancelled cutter compensation will recover by the buffered next compensation plane block.
Note: In the compensation mode, the bit 2 of parameter No.:42 can be selected that when G28 or G30 code moves at
the intermediate point, and then confirm whether the compensation will dwell temporarily.
Cutter compensation cancellation (G40)
In the G00, G01 state, the following code is used, G40 X__ Y__;
The linear operation from the old vector of start to the end is performed. In the G00 mode, each
axis moves to the end at the rapid traverse rate. The system enters the tool compensation
cancellation state from the tool compensation state when using this code.
Tool will never operate when X__ Y__ does not specify but the G40.
Cutter compensation
Left (G41)
1) G00, G01
G41 X__ Y__ D__; code locates at the end of block and forms a new vector vertical with
the (X, Y) directin, tool moves to the point of new vector from the old one at the start.
New r
vecto
(X,Y)
Tool center path
e c to r
O ld v
Start
Programming
path
Fig. 4-7-2-2
Using this code when old vector is regarded as 0, so that the tool enters to the cutter
121
VOLUME I
PROGRAMMING
position; the axie other than the tool radius offset axis does not cancel. When G53 is shared a
GSK218MC Series Machining CNC System
Programming & Operation Manual
compensation state from the tool offset cancellation state. In this case, the offset value is
specified by D code.
2) G02, G03
G41……；
……
……
G02 /G03 X__ Y__ R__ ;
New vectors can be carried out by the above-mentioned programs, which are located at the
line between arc center and end; viewing from the forward direction of the arc, point at the left (or
right); tool center moves along arc from the old vector point of arc to the new one. However, the
premise is that the old vector has been performed correctly.
VOLUME I
PROGRAMMING
The offset vector points to the arc center or departs from the center from the start or end.
New vector
Tool center
path
(X,Y)
Programming
path
R
New
vector
(X,Y)
R
Tool center path
Old vector
Start
Old vector
Programming
path
Start
Fig. 4-7-2-3
Cutter compensation
Right (G42)
G42 is opposite to G41, which moves forward along the tool, and the tool offsets at the right of
workpiece. That is, the vector direction from G42 is opposited to the one of G41; however the offset
method is absolute identical with the G41 other than the vector direction.
1) G00, G01
G42 X__ Y__ D__ ；
G42 X__ Y__ ；
(X,Y)
Programming path
Start
Ol d v
ector
Tool center path
Fig. 4-7-2-4
122
Ne w r
vecto
Chapter Four
Preparatory Function G Code
2) G02, G03
(X,Y) New vector
(X,Y)
Programming
path
New vector Programming
path
R
Start
R
Tool center
Start
path
Old vector
Tool center path
Fig. 4-7-2-5
(A) The specification of offset
G41, G42 and G42 are modal codes of which the offset numbers are specified by G code. Any
position can be specified before the cutter compensation state from offset state cancellation.
(B) Enter the cutter compensaton state from the offset state cancellation
The movement codes from offset state cancellation to the cutter compensation state should be
performed the positioning (G00) or linear interpolation (G01) instead of using the arc interpolation
(G02, G03).
(C) The shifting between the cutter compensation left and right
Generally, whenever the offset direction performs from left to right or on the contrary, which goes
throught the offset cancellation state. However, the positoning (G00) or linear interpolation (G01) can
be directly shifted instead of passing the offset cancellation state. In this case, the tool path is as
follows:
Tool center path
(Generally, it is not straight line)
Old
r
vecto
Start
Programming
path
Programming
path
(X,Y)
N ew
r
vecto
Start
Old
r
vecto
N ew
r
vecto
(X,Y)
Tool center path
(Generally, it is not straight line)
Fig. 4-7-2-6
G1G41 D__X__ Y__；
……
G1G42 D__X__ Y__；
G42 D__X__ Y__；
……
G41 D__ X__ Y__；
(D) The alteration of offset value
123
VOLUME I
PROGRAMMING
6. The common precautions for the offset:
GSK218MC Series Machining CNC System
Programming & Operation Manual
The alteration of offset value, generally, is in the offset cancellation state, when the tool-change
performs, the position (G00) and linear interpolation also can be performed in the offset state, its
description is shown below:
Tool center path
Tool center path
New
r
vecto
(X,Y)
r
vecto
New
(X,Y)
ector
Old v
Programming
path
Old v
ector
Programming
path
Start
Start
Fig. 4-7-2-7 (The alteration of offset vector)
VOLUME I
PROGRAMMING
(E) The +/- of offset value and tool center path
If the offset value is set as negative value, the machined workpiece equals to that the G41 and
G42 on the program list are totally changed. And therefore, the cutting along the external workpiece
becomes to the internal cutting, and the original internal machinig along workpiece turns into the
external machining.
It is supposed that the offset value is positive value in the common program; refer to the following
figure:
When the offset value of the tool path programming (Fig. A) is set as negative value, so that the
tool movement path is as the Fig. B; similarly, if the offset value of the tool path programming (Fig. B)
is set as negative value, and then the tool movment path is as the Fig. (A).
Tool center path
Tool
Tool
Fig.（A）
Programming
path
Fig.（B）
Fig. 4-7-2-8
Generally, the figure with the pointed angle is the most common. However, after the offset value
is set to negative value, the inner round of machining component can not be performed. When an
inner pointed angle of one angle is cut, inser the sutiable radius arc at this position, and then the
cutting can be performed after the acr transition.
Whether it is the left compensation or the right is confirmed that the tool movement is left or right
roleated to the workpiece (it is regarded as the workpiece unmoved). The system enters the
124
Chapter Four
Preparatory Function G Code
compensatin mode by G41 or G42 and cancels it by G40.
The example of compensation program shows below:
The block (1) calls starting, the compensation cancellation mode in the block becomes
compensation mode by G41. At the end of this block, tool center is vertical to the compensation
direction of the next program path (From P1 to P2) by tool radius. The tool compensation value is
specified by D07, that is, the compensation number is set to 7, and the G41 means the tool path path
compensation left.
The tool path compensation is automatically performed after the compensation starts and when
the workpiece shape is compiled such as P1→P2……P9→P10→P11.
The program example of tool path compensation:
G92 X0 Y0 Z0；
VOLUME I
PROGRAMMING
(1) N1 G90 G17 G0 G41 D7 X250 Y550 ； (The compensation value should be set by its
compensation number in advance.)
(2) N2 G1 Y900 F150 ；
(3) N3 X450 ；
(4) N4 G3 X500 Y1150 R650 ；
(5) N5 G2 X900 R-250 ；
(6) N6 G3 X950 Y900 R650 ；
(7) N7 G1 X1150 ；
(8) N8 Y550 ；
(9) N9 X700 Y650 ；
(10) N10 X250 Y550 ；
(11) N11 G0 G40 X0 Y0 ；
5
250R
C1(700,1300)
P5(900,1150)
650R
650R
P4(500,1150)
6
4
3
P6(950,900)
P2(250,900)
C2(1150,1550)
7
P7
P3(450,900)
(1150,900)
2
8
P9(700,650)
(1150,550)
(250,550)
P
P
10
9
Y axis
1
11
Start (Program origin)
X axis
Fig. 4-7-2-9
125
GSK218MC Series Machining CNC System
4.7.3
Programming & Operation Manual
Details of Cutter Compensation
Concept: Inner side and outer side: When an angle of intersection created by tool paths specified
with move command for two blocks in over 180°, it is referred to as “inner side.” When the
angle is between 0° and 180°, it is referred to as “outer side.”
Inner side
Workpiece
Outer
side
α
Programmed path
α
VOLUME I
PROGRAMMING
Programmed path
Workpiece
α≥180°
180°≥α≥0
Fig. 4-7-3-1
The meaning of symbols:
The following symbols are used in sebsequent figures:
―― S indicates a position at which a single block is executed once.
―― SS indicates a position at which a single block is executed twice.
―― SSS indicates a position at which a single block is executed thrice.
―― L indicates that the tool moves along a straight line.
―― C indicates that the tool moves along an arc.
―― r indicates the cutter compensation value
―― An intersection is a position at which the programmed paths of two blocks
intersect with each other after they are shifted by r.
―― O indicates the center of the tool
1. Tool movement in start-up When the offset cancellation mode is changed to offset mode, the
tool moves as illustrated below (Start-up):
126
Chapter Four
Preparatory Function G Code
(a) Tool movement around an inner side of a corner (α≥180°)
Linear - Linear
Linear - Arc
α
α
G42
r
S
Start
Programming
path
G42
r
S
L Tool center path
L
C
Programming
path
L
Start
Tool center path
Tool path in the beginning of compensation has two types A and B, which are selected by bit 0
of parameter No.: 40:
Linear - Linear
Start position
Linear - Arc
Start position
G42
G42
α
Programmed
path
L
r
A
S
α
L
r
L
Tool center path
Programmed path
Programmed
path
S
C
Tool center path
B
(C) Tool movement around the outside of an acute (α＜90°）
Tool path in the beginning of compensation has two types A and B, which are selected by bit 0
127
VOLUME I
PROGRAMMING
(b) Tool movement around the outside of a corner at an obtuse angle (180°＞α≥90°)
GSK218MC Series Machining CNC System
Programming & Operation Manual
of parameter No.: 40:
Linear—Linear
Linear—arc
Start
Start
G42
G42
α
α
L
r
A
Programmed
path
L
S
VOLUME I
PROGRAMMING
L
S
B
C
Linear－Arc
Linear－Linear
L
S
G42
G42
L
α
Programmed
path
r
L
Programmed
path
S
Tool center path
Tool center path
L
L
r
L
α
r
L
L
C
Tool center path
Tool center path
Programmed
path
(d) Tool movement around the outside linear→linear at an acute angle. (α＜1°)
S
L
Tool center path
L
r
Programmed
path
G41
Less than 1º
Fig. 4-7-3-2
2. Tool movement in offset mode
The invariable compensation plane is performed in the compensation mode; otherwise, the
alarm may issue, and the tool stops at the same time. In the offset mode, the movement of tool is as
follows:
128
Chapter Four
Preparatory Function G Code
(a) Tool movement around the inside of a corner (α≥180°)
L in e a r
L in e a r
Linear
Arc
α
α
P ro g ra m m e d
p a th
S
L
In te rs e c tio n
S
C
Intersection
T o o l c e n te r p a th
L
Tool center
path
L
Arc
Program m ed
path
Linear
Arc
Arc
α
Program m ed
path
C
S
Intersection
L
Tool center
path
L
S
Intersection
C
Tool center
path
Programmed
path
Fig. 4-7-3-3
3. When it is exceptional
There is no intersection of the
compensation value of circular arc
when tool radius value is small,
refer to the left figure; however,
when the tool radius is becomes
bigger, the intersection may be
inexistent, and the system
displays the alarm “Interference
exists in the cutter compensation
C”.
(I) There is no intersection
Alarm & stop
When compensation
value is large
When compensation
value is small
Programmed path
Fig. 4-7-3-4
4. The tool movement in offset cancellation mode
In the compensation mode, when any of the following items of the block is performed; the system
then enters the compensation cancellation mode, and the movement of the block is called
Compensation cancellation.
a) Code G40
b) Cutter compensation number is 0.
Fail to use the arc code (G03 and G02) to cancel when the compensation cancellation is
performed, if the commanded arc may alarm and tool may stop.
129
VOLUME I
PROGRAMMING
α
GSK218MC Series Machining CNC System
Programming & Operation Manual
(a) Tool movement around the inside of a corner (α≥180°)
Linear→Linear
Arc→Linear
α
α
Programmed path
r
r
G40
Tool center path
L
G40
C
S
L
S
Programmed
Tool center path
path
L
VOLUME I
PROGRAMMING
(b) Tool movement around the inside with a corner (90°≤α<180°)
Tool path in the beginning of compensation has two types A and B, which are selected by bit
0 of parameter No.: 40:
Arc—Linear
Linear—Linear
Programmed
path
Programmed
path
C
Tool center path
S
Tool center
path
S
A rc
Linear
L
r
L
r
L
A
G40
α
G40
α
L in e a r
Linear
α
G40
α
Programmed
path
B
L
Tool center path
r
S
Intersection
r
L
L
S
In te r s e c tio n
C
P ro g ra m m e d
T o o l c e n te r p a th
p a th
(c) Tool movement around the outside with an acute angle (α< 90°)
Tool path in the beginning of compensation has two types A and B, which are selected by bit
0 of parameter No.: 40:
130
Chapter Four
Preparatory Function G Code
Linear — Linear
Arc — Linear
G40
G40
α
Programmed
α
path
Programmed
path
L
A
L
Tool center path
r
L
r
L
Tool center
path
Linear-Linear
Programmed
h
r
G42
L
α
L
L
S
G42
L
VOLUME I
PROGRAMMING
L
S
B
Linear-Circular
α
r
L
Programmed path
Tool center path
Tool center path
C
(d) Tool movement around the inside (α＜1°) with an obtuse angle, linear → linear
L
Tool center path
S
L
Programmed path
r
G42
α less than degree
G40
Fig. 4-7-3-5
5. Alter the compensation direction in the compensation mode
The compensation direction is determined by cutter compensation G code (G41 and G42), the
symbol of compensation value is shown below:
Table 4-7-3-1
Sign of compensation value
+
-
G41
Left compensation
Right compensation
G42
Right compensation
Left compensation
G code
131
GSK218MC Series Machining CNC System
Programming & Operation Manual
In the special occasion, the compensation direction can be changed in the compensation mode
instead of altering at the beginning of stat and its subsequent blocks. When the compensation
direction changes, there is no inner side and outer side. It is supposed to positive for the following
compensation value.
(i) Linear—>Linear
(ii) Linear—>Arc
S
L
G42
C
ｒ
ｒ
L
L Tool center path S
VOLUME I
PROGRAMMING
(iv) Arc—>Arc
Tool center path
G42
G42
L
ｒ
ｒ
G41
C
G41
G42
ｒ
Tool center path
(iii) Arc—>Linear
ｒ
Programmed path
G41
Programmed
path
ｒ
S
Tool center path
ｒ
Programmed
path
C
Programmed
path
C
G41
S
Fig. 4-7-3-6
(V) If the compensation is normally performed but there is no intersection
When the offset direction blocks A and B are changed by G41 and G42, if there is no need any
intersection of compensation path, the start at the block B is vertical to the vector of the block B.
(1) Linear-----Linear
S
Programmed
path
Tool center
path
Block A
(G42)
(G42)
L
S
L Compensation
vector
Fig. 4-7-3-7
132
L
Block B
(G41)
Chapter Four
Preparatory Function G Code
(2) Linear-----Arc
S
L
(G41)
Block A
Tool center
path
(G42)
Block B
Programmed (G41)
path
Compensation
vector
C
VOLUME I
PROGRAMMING
Fig. 4-7-3-8
(3) Arc-----Arc
C
S
Block A
(G42)
(G42)
r
Programmed
path
r
S L
C
L
r
Block B
(G41)
The end point
is out of arc
Cneter
Tool center
path
Center
Fig. 4-7-3-9
(vi) When the cutter compensation
(vi) Generally, the following decription will not occur when cutter compensation makes the tool center
path length above one circle. However, the following conditions may be generated when G41 and
G42 are charge.
Arc—Arc (Linear—Arc)
The system will alarm when cutter compensation changes its
direction; the alarm prompts “Arc code can not cancel the tool compensation!” when tool
number is regarded as D0.
Linear – Linear
Tool compensation direction can be altered.
133
GSK218MC Series Machining CNC System
Tool center path
(G42)
N5 G01 G91 X500 Y-700;
N6 G41 G02 J-500;
N7 G42 G01 X500 Y700;
In this case, tool center path is
not an arc instead of section arc
from P1 to P2. In some
conditions, the alarm may be
checked out due to the
interference.
If we hope that the tool moves
along the whole circle, it is
necessary to specify it with
section.
Programmed
path
N7
N5
P2
P1
Programming & Operation Manual
N6
Fig. 4-7-3-10
6. Compensation cancellation in dwell
VOLUME I
PROGRAMMING
In the compensation mode, when the G28, G30 code can be specified by bit 2 of parameter No.:
40, whether the compensation is cancelled temporarily at the intermediate point.
a) G28 automatic reference position return
In the compensation mode, if the G28 is commanded, and the compensation will be
cancelled at the intermediate point; the compensation mode is automatically recovered after the
reference position is turned.
G28
S
r
(G00)
S
r
(G42 G00)
S Origin
Programmed Tool center
path
path
Fig. 4-7-3-11
b) G29 automatically returns from reference origin
In the compensation mode, if the G29 is specified, and the compensation will be cancelled
at the intermediate point; the compensation mode is automatically recovered when returning the
specified point by G29.
Immediately specify it followed with G28
G28 Intermediate
point
S
r
(G42 G00)
Programmed
path
S
r
S
S
G29
Tool center path
Fig. 4-7-3-12
134
(G00)
S Origin
Chapter Four
Preparatory Function G Code
It does not immediately specify it followed with G28:
G29
Intermediate
point
S
r
S
r
(G42 G00)
S
(G00)
Programmed
Tool center path
path
Fig. 4-7-3-13
When specifying the cutter compensation G codes (G41, G42) in the compensation mode, it
becomes a rectangular vector with the previous block related to the movement direction and it
regardless of the machining inner side and outer side. However, if this G codes are specified in arc
code, the correct arc can not be gained accordingly.
When the cutter compenatin G codes (G41, G42) are changed the compensation direction, refer
to the (5).
Linear-----Linear
Programmed G42 mode
path
r
L
Tool center path
r
G42 command
block including
r
S
L
Fig. 4-7-3-14
Arc-----Linear
135
VOLUME I
PROGRAMMING
7. Cutter compensation G code in compensation mode
GSK218MC Series Machining CNC System
r
Programming & Operation Manual
G42 command
block including
r
G42 mode
S
L
C
Programmed
path
Tool center path
Fig. 4-7-3-15
VOLUME I
PROGRAMMING
8. A block without tool movement
There is no tool movement in the following blocks. In the blocks, it will not move even if the cutter
compensation mode is enabled.
(1) M05 ； …………………… M code output
(2) S21 ； …………………… S code output
(3) G04 X10； ……………
Dwell
(4) (G17) Z100 ；……………… Without movement code inside the compensation plane
(5) G90 ；……………………… G code only
(6) G01 G91 X0； …………… Movement value is 0
a) The code at the beginning of compensation
The system will generate start-up operation at the next movement code if the start-up block
does not move.
N7
SS
S
N6
N8
Tool center path
r
Programmed
path
N9
G40 G91……
.
.
N6 X100 Y100;
N7 G41 X0;
N8 Y-100;
N9 X100 Y-100;
Fig. 4-7-3-16
b) In the compensation mode command
When only one block without tool movement is specified in compensation mode, the vector
and the tool center path is same as that when the command does not specify. (Refer to the item
136
Chapter Four
Preparatory Function G Code
(3) compensation mode). In this case, the block without tool movement is performed at the single
block stop position.
N8
N7
N6 G91 X100 Y200;
N7 G04 X100;
N8 X100;
SS
N6
Block N7
performs here
Programmed
path
Tool center path
Fig. 4-7-3-17
more blocks of without tool movement are commanded even if only one block is specified.
N8
N7
N6 G91 X100 Y200;
N7 X0;
N8 X100;
SS
N6
Block N7
performs here
Programmed
path
Tool center path
Fig. 4-7-3-18
Note: The above-mentioned block is operated based upon the G1, G42, the path is inconsistent with the figure in G0.
c) It is specified with the compensation cancellation together
When there is no tool movement of a block specified with the compensation cancellation
together, it may form the length compensation, and its direction is vertical to the movement direction
vector of the previous block, and this vector will be cancelled at the next command.
N8
N7
N6 G91 X100 Y100;
N7 G40;
N8 X100 Y0;
r
SS
N6
Programmed
path
Tool center path
Fig. 4-7-3-19
137
VOLUME I
PROGRAMMING
However, when the movement value is zero, tool motion becomes the same as that when two or
GSK218MC Series Machining CNC System
Programming & Operation Manual
9. Corner movement
When more than two vectors are produced at the end of a block, the tool moves linearly from one
vector to another. This movement is called the corner movement.
If ΔVX≤ΔV limit and ΔVY≤ΔV limit, the latter vector is ignored.
If these vectors do not coincide, a movement is generated to turn around the corner, which
belongs to the previous block.
These motions are belonged to the
block N6, thus, the feedrate equals to
that in block N6. If the block N6 is G00
Mode, the tool is moved at the rapid
traverse rate; if the block N6 is G01,
G02 and G03 modes, the tool is moved
based upon the cutting feedrate.
S
VOLUME I
PROGRAMMING
N7
N6
Fig. 4-7-3-20
However, if the path of the next block is semicular or more, the above-mentioned function is not
performed; and its reason is as follows:
P2 (P3,P4) P5
P1
Tool center
path
N5
N7
N4 N8
P7
P0
Programmed
path
P6
N4
N5
N6
N7
N8
G41 G91 X150 Y200;
X150 Y200;
G02 J-600;
G01 X150 Y-200;
G40 X150 Y-200;
N6
Fig. 4-7-3-21
If the vector is not ignored, the tool path is as follows:
P0 →P1 →P2 →P3 (circular arc) →P4 →P5 →P6 →P7
But if the distance between P2 and P3 is negligible, the point P3 is then omitted. Therefore, the
tool path is as follows:
P0 →P1 →P2 →P4 →P6 →P7 The arc cutting of block N6 is ignored.
138
Chapter Four
Preparatory Function G Code
10. Interference check
Tool overcutting is called interference. The interference can check the tool overcutting in
advance. If the interference is checked in the syntax inspection after loading the program, the system
will then alarm. Whether the interference check is performed when the bit 6 of parameter No.: 41 is
set the radius compensation.
The basis conditions of interference:
(1) The movement distance of the block for establishing the cutter compensation is less than
tool radius.
(2) The tool path direction defers from the programmed path direction. (The angle of path
between the 90° and 270°).
(3) When the arc machining is performed, the angle of its start and end of tool center path is
VOLUME I
PROGRAMMING
great different to the one of the programmed path (more than 180°).
Programmed path
Tool center
path
Great different
between two
path directions
(180°)
Fig. 4-7-3-22
Tool center
path
Programmed
path
Great different
between two path
directions (180°)
Fig. 4-7-3-23
11. Manual operation
The manual operation in tool point radius compensation, refer to the manual operation in the
139
GSK218MC Series Machining CNC System
Programming & Operation Manual
Volume Operation.
12. The general precautions for compensation
a) Command compensation value
The compensation value is specified the compensation value number by D code. The D
code is always enabled till another one is specified or cancelled the compensation once it is
specified. D code, also, is not only used for specifying the compensation value to the cutter
compensation but also for the offset value of tool offset.
b) Compensation value alteration
Usually, when the tool-change is performed, the compensation value should be altered in
the cancellation mode. If the compensation value is changed in the compensation mode, a
VOLUME I
PROGRAMMING
new compensation value will be calculated at then end of the block.
Compensation
value
calculation in
block N6
Compensation
value
calculation in
block N7
N7
N8
N6
Programmed
path
Fig. 4-7-3-24
c) The +/- of compensation and tool center path
The G41 and G42 in the program will be exchanged if the compensation value is negative (-).
If the tool center moves along the workpiece outer side, the compensation value may move
along the inner side, vice versa.
The following figure shows that the compensation value is (+) when the program is
performed. When the tool path (Fig. a) is programmed, if the compensation value is negative (-),
and the tool center moves as (Fig. b), vice versa. Therefore, the male form or female form can be
cut at the same program, and its interval can be adjusted by the comensation value.
Tool center path
Tool
Tool
Fig (a)
Programmed path
Fig. 4-7-3-25
140
Fig. (b)
Chapter Four
Preparatory Function G Code
d) Overcutting by cutter compensation
(1) When the machining is performed by the arc less than the tool radius
When the corner radius is less than the cutter radius, the internal compensation of the
cutter will result in overcutting, therefore, the interference may alarm and stop before
performing.
Tool center
path
The interference alarm
occurs before operating, the
operation is then stopped.
Programmed
path
Normally, do not
perform the
interference inspection
over-cutting path
VOLUME I
PROGRAMMING
The over-cutting may occur if the CNC does not stop.
Fig. 4-7-3-26
(2) Machining groove smaller than the tool radius
When the machining is performed by the cutting-groove less than the tool radius, the cutter
compensation forces the tool center path that moves along the negative direction of
programmed path; the overcutting then may occur.
Tool center
path
Alarm occurs,
operation stops
Programmed
path
The over-cutting may occur if the CNC does not stop.
Fig. 4-7-3-27
141
GSK218MC Series Machining CNC System
Programming & Operation Manual
(3) Machining section-difference smaller than the tool radius
If the section-difference smaller than the tool radius performs in program, and when the
machining of this section-difference is specified by arc machining, the normal tool center path of
compensation then becomes opposite to the program direction. In this case, the initial vector is
omitted, and the tool moves to the 2nd vector linearly. Single block stops here. The automatic
operation may continue if the machining is performed regardless of the single mode. If the
section-difference is straight line, the alarm will not issue instead of cutting correctly, but the end
of cutting section may be remained.
Single block end
Linear movement
S
VOLUME I
PROGRAMMING
Tool center
path
Programmed
path The over-cutting may
occur if the initial vector
does not omit.
Arc center
The initial vector is
omitted.
Fig. 4-7-3-28
Cutter compensation start and movement along the Z axis
Generally, when the machining is started and after the cutter compensation is enabled, tool
moves a section of distance from the workpiece along with Z axis. If the movement along the
Z axis is divided into rapid feed and cutting feed based upon the above-mentioned
conditions, refer to the following programs:
If it is the block N3 (movement code along Z axis)
It is divided into as the follows:
N1 G91 G00 G41 X500 Y500 D01;
N3 Z-250;
N5 G01 Z-50 F1;
N6 Y100 F2;
Fig. 4-7-3-29
142
Chapter Four
4.7.4
Preparatory Function G Code
Corner Offset Arc Interpolation (G39)
Format:
G39
Function: By specifying G39 in offset mode during cutter compensation, corner offset circular arc
compensation can be performed. The radius of corner compensation equals to the
compensation value. Whether the corner arc in the radius compensation is enabled by
setting the bit 5 of parameter No.: 41.
Explanation:
1. When the G39 code is specified, corner arc interpolation in which the radius equals to the
compensation value can be performed.
one-shot G code.
3. When G39, is programmed, the arc at the corner is formed so that the vector at the end
point of the arc is perpendicular to the start point of the next block. Refer to the following
figure:
.
.
(In offset mode)
.
N1 X10;
N2 G39;
N3 Y-10;
.
.
.
Block N1
Y
X
Block N2
Tool center path
Programmed
path
Offset vector
（10，0）
Block N3
（10，-10）
Fig. 4-7-4-1
4.7.5
G39
Tool Compensation Value, Entering Compensation Number From
Program (G10)
Format:
G10 L10 P_ R_ ;
Geometric compensation value of H code
G10 L12 P_ R_ ;
Geometric compensation value of D code
G10 L11 P_ R_ ;
Wear compensation value of H code
G10 L13 P_ R_ ； Wear compensation value of D code
143
VOLUME I
PROGRAMMING
2. G41 or G42 preceding the code determines whether the arc is CW or CCW, G39 is
GSK218MC Series Machining CNC System
Programming & Operation Manual
P : Tool compensation number.
R : Tool compensation value in the absolute value code (G90).
Tool compensation value in the absolute value code (G91) adds the value of the
specified tool compensation number (The sum is tool compensation value)
Explanation: Available input range of tool compensation value:
Geometric
compensation:
metric
input
-999.999mm~+999.999mm;
Inch
input
-39.3700inch~+39.3700inch.
Wear compensation: metric input -400.000mm~+400.000mm (Evaluate the No.267 data
parameter setting); Inch input -39.3700inch~+39.3700inch (Evaluate 1/25.4 of
the No.267 data parameter setting).
Note 1: The maximum value of the wear compensation is restricted by data parameter P267.
VOLUME I
PROGRAMMING
4.8 Feed G Code
4.8.1
Feed Mode G64/G61/G63
Format:
Exact stop G61
Tapping mode G63
Cutting mode G64
Functions:
Exact stop method G61: This function is always enabled once specifying before G62, G63 or
G64 is specified. Tool decelerates and performs in-position detection at the end
of the block, and then perform the next block.
Tapping method G63: This function is always enabled once specifying before G61, G62 or G64
is specified. Tool does not decelerate instead of executing next block at the end
of the block. When specifying G63, both the feedrate override and feed hold are
disabled.
Cutting method G64: This function is always enabled once specifying before G61, G62 or G63
is specified. Tool does not decelerate instead of executing next block at the end
of the block.
Explanations:
1. Without parameter format.
2. G64 is the default feed mode of the system; the end of the block does not decelerate
instead of executing next block.
3. The destination of the in-position detection in exact mode is check whether the servo motor
is reached within the specified position range.
144
Chapter Four
Preparatory Function G Code
4. In the exact stop mode, the tool paths are different between the cutting and tapping methds.
Refer to the following Fig. 4-8-1-1
Y
Position check
(2)
Tool path in exact stop mode
(1)
Tool path in the cutting or tapping mode
X
0
Fig. 4-8-1-1 Tool path from block 1 to block 2
VOLUME I
PROGRAMMING
4.8.2
Automatic Corner Override (G62)
Format: G62
Function: Once the Auto corner override method G62 is specified, this function is always enabled
before G61, G62 or G63 is specified. When the tool moves along the inner corner during the
cutter compensation, the cutting feed override is performed to restricting the cutting value
within the unit time; in this case, the fine surface accuracy can be machinined accordingly.
Explanatins:
1. When cutter compensation is performed, the movement of the tool is automatically
decelerated and reduced the load on the cutter at an inner corner and internal circular arc
area, so that it produces a smoothly machined surface.
2. Whether the automatic corner override function is available is set by bit 7 of parameter No.:
16. Control the automatic corner deceleration function (0: Angle control, 1: Speed difference
control) by bit 2 of parameter No.: 15.
3. When specifying G62 and machining inner corner with cutter compensation function,
automatically adjust the feedrate both ends of corner. There are four inner corners, refero to
Fig. 4-8-2-1; wherein, 2°≤θ≤θp≤178°; θp is set by data parameter P144.
145
GSK218MC Series Machining CNC System
：Tool
1. Straight line - Straight line
Programming & Operation Manual
2. Straight line - Arc
：Programmed path
：Tool center path
4. Arc - Arc
3. Arc – Straight line
VOLUME I
PROGRAMMING
Fig. 4-8-2-1
4. When a corner is determined to be an inner corner, the feedrate is overridden before and
after the inner corner. The distances Ls and Le, where the feedrate is overridden, are
distances from the points on the cutter center path to the corner. Refer to 4-8-2-2, wherein,
Ls+Le≤2mm.
Le
a
Programmed
path
Tool center path
Ls
b
The feedrate is overridden
from point a to b.
Fig. 4-8-2-2
Straight line to straingt line
5. When a programmed path consists of two arcs, the feedrate is overridden if the start and
end points are in the same quadrant or in adjacent quadrants. The lowest feedrate is
decelerated by controlling automatic corner using data parameter P145, refer to the Fig.
4-8-2-3.
146
Chapter Four Preparatory Function G Code
Programmed
path
a
Le
Ls
b
Tool center
path
The feedrate is overridden from point a to b.
Fig. 4-8-2-3
Arc to arc
feedrate is overridden from point a to b and from c to d. Refer to the Fig. 4-8-2-4.
d
Le Ls
Programmed
path
a
Le Ls
b
c
Tool
Tool
Tool center path
Fig. 4-8-2-4 Straight line to arc, arc to straight line
Limitations:
1. Override for inner corner is disabled during acceleration/deceleration before
interpolation.
2. Override for inner corner is disbled if the corner is preceded by a start-up block or
followed by a blocking including G41 or G42.
3. Inner cornder is not performed if the offset is zero.
4.9 Macro Function G Code
4.9.1
User Macro Program
One function carried out by one group code is registered to memory in advance, like subprogram.
This functions can be indicated by one code, which can be performed only write the represented code
147
VOLUME I
PROGRAMMING
6. Regarding a program is both from straight line to arc and from arc to straight line; the
GSK218MC Series Machining CNC System
Programming & Operation Manual
in program. The group codes are called user macro program body, and the represented codes are
regarded as “User Macro Code”. The user macro program body, sometimes, is abbreviated as Marco
Program, and the user macro code is also treated as Macro program call code.
User macro
program body
Main
program
Complete a group
of command of
one function
User macro
program command
VOLUME I
PROGRAMMING
Fig. 4-9-1-1
The variable can be used in user macro program body. The calculation can be performed among
variables, and the variable also can be assigned by macro code.
4.9.2
Macro Variable
Both the common CNC command and the variable, as well the calculation and code shifting can
be used in user marco program.
User macro program ends by M99 from the beginning of program number.
O0066;
Program number
G65 H01 ……；
Calculation command
G90 G00 X#101 ……； CNC command used
with variable
……
……
……
G65 H82 ……；
Command shifting
……
……
M99;
User macro program body end
Fig. 4-9-2-1 The composition of user macro program body
1. Usage of variable
The parameter value in user macro program body can be specified by variable. The variable
148
Chapter Four Preparatory Function G Code
value can be assigned by main program or set by LCD/MDI, as well, evaluate the value to be
calculated when performing the user macro program body.
Multiple variables can be used, which can be distinguished from variable number.
(1) The indication of variable
The variable can be indicated by the consecutive variable number followed with #, the format
shows below:
#i (i = 1, 2, 3, 4 ……)
(For example) #5， #109， #1005
(2) The quotation of variable
The numerical value followed with the parameter can be replaced by variable.
(For example) F#103
When #130 = 3, it is same as the G3.
Notice: 1. Parameter word O and N (Program number and Seqence number) can not be quoted the variable. And it
can not be programmed by O#100, N#120.
2. It can not be used if exceeds the top code value specified by parameter value. When #30 = 12, M#30
exceeds the Max. code value.
3. The display and setting of variable value: The variable value can be displayed on LCD and set by MDI
mode.
2. Types of variable
Variable can be divided into null, local, common and system variables, which are different in the
purpose and character.
(1) Null variable #0: (This variable is always null, no value can be assigned to this variable)
(2) Local variable #1～#50: Local variables can only be registered the data in macro program;
bit 7 of parameter No.: 52 can be reset or whether it is eliminated after ESP. When a macro program
is called, arguments are assigned to local variables.
(3) Common variables #100～#199, #500～#999: Bit 6 of parameter No.:52 can be reset or
whether it is eliminated the common variables #100～#199 after ESP.
Common variables are public one in main program and each user macro program called by main
program; that is, the used variable #i in one user macro program is identical with the one of other
macro programs. Therefore, the common variable #i in one macro program calculation result can be
used in other macro programs.
The purpose of common variable does not specify in system, user can be used it freely.
Table 4-9-2-1
Variable number
＃100～＃199
Variable type
Common
variable
Function
The variable numbers are eliminated when
the power is turned off and reset to “Null”
when the power is turned on.
149
VOLUME I
PROGRAMMING
G#130
When #103 = 15, it is identical with the F15 command.
GSK218MC Series Machining CNC System
＃500～＃999
Programming & Operation Manual
The data are registered in file, and they will
not absent even if the power is turned off.
(4) System variables: System variables are used to read and write a variety data when CNC is
performed, which are separately shown below:
1) Interface input signal #1000 --- #1015 (Read PLC based upon the bit and input the signal to
system, that is G signal)
#1032 (Read PLC based upon byte and input the signal to system,
that is G signal)
2) Interface output signal #1100 --- #1115 (Write system output based upon bit to the signal of
PLC, that is F signal)
VOLUME I
PROGRAMMING
#1132 (Write system output based upon byte to the signal of PLC,
that is F signal)
3) Tool length compensation value #1500 --- #1755 (Read-write)
4) Length wear compensation value #1800 --- #2055 (Read-write)
5) Cutter compensation value #2100 --- #2355 (Read-write)
6) Radius wear compensation value #2400 --- #2655 (Read-write)
7) Alarm
8) User data table
#3000
#3500 --- #3755 (Read only)
9) Modal information #4000 --- #4030 (Read only)
10) Position information
#5001 --- #5030 (Read only)
11) Workpiece zero offset value 5201 --- #5235 (Read-write)
12) Additional workpiece coordinate system #7001 --- #7250 (Read-write)
3. The details of system variable
1) Modal information
Table 4-9-2-2
Variable
Function
Group No.
#4000
G10,G11
Group 00
#4001
G00,G01,G02,G03
Group 01
#4002
G17,G18,G19
Group 02
#4003
G90,G91
Group 03
#4004
G94,G95
Group 04
#4005
G54,G55,G56,G57,G58,G59
Group 05
#4006
G20,G21
Group 06
#4007
G40,G41,G42
Group 07
#4008
G43,G44,G49
Group 08
No.
150
Chapter Four Preparatory Function G Code
G22,G23,G24,G25,G26
#4009
G32,G33,G34,G35,G36,G37,G38
Group 09
G73,G74,G76,G80,G81,G82,G83,G84,G85,G86,G87,G88,G89
G98,G99
Group 10
#4011
G15,G16
Group 11
#4012
G50,G51
Group 12
#4013
G68,G69
Group 13
#4014
G61,G62,G63,G64
Group 14
#4015
G96,G97
Group 15
#4016
To be extended
Group 16
#4017
To be extended
Group 17
#4018
To be extended
Group 18
#4019
To be extended
Group 19
#4020
To be extended
Group 20
#4021
To be extended
Group 21
#4022
D
#4023
H
#4024
F
#4025
M
#4026
S
#4027
T
#4028
N
#4029
O
#4030
VOLUME I
PROGRAMMING
#4010
P (The additional workpiece coordinate system selection at
present)
Note 1: The P code is the selected additional workpiece coordinate system at present.
Note 2: When performing G#4002, the value gained from #4002 is 17, 18 or 19.
Note 3: Modal information can not be wrote, which is read only.
2) Current position information
Table 4-9-2-3
Variable
No.
#5001
#5002
Position Information
Relevant
Read
Tool
Coordinate
Operation
Compensation
System
in Moving
Value
Block end position along X
Workpiece
axis (ABSIO)
coordinate
Block end position along Y
system
axis (ABSIO)
Can
Take no
consider of the
tool point
position
151
GSK218MC Series Machining CNC System
#5003
#5004
#5006
#5007
#5008
Programming & Operation Manual
Block end position along Z
(program
axis (ABSIO)
specified
Block end position along 4th
position)
axis (ABSIO)
Block end position along X
axis (ABSMT)
Block end position along Y
Machine
axis (ABSMT)
tool
Block end position along Z
coordinate
axis (ABSMT)
system
th
VOLUME I
PROGRAMMING
#5009
#5011
#5012
#5013
#5014
#5016
#5017
#5018
#5019
#5021
#5022
#5023
#5024
#5026
152
Block end position along 4
axis (ABSMT)
Can not
Block end position along X
axis (ABSOT)
Conside of the
Block end position along Y
tool reference
axis (ABSOT)
point position
Block end position along Z
(Machine
axis (ABSOT)
Block end position along 4th
axis (ABSOT)
Block end position along X
axis (ABSKP)
coordinate)
Workpiece
coordinate
system
Block end position along Y
axis (ABSKP)
Block end position along Z
Can
axis (ABSKP)
Block end position along 4th
axis (ABSKP)
Tool length compensation
value along X axis
Tool length compensation
value along Y axis
Tool length compensation
value along Z axis
Tool length compensation
value along 4th axis
Servo position compensation
along X axis
Can not
Chapter Four Preparatory Function G Code
#5027
#5028
#5029
Servo position compensation
along Y axis
Servo position compensation
along Z axis
Servo position compensation
along 4th axis
Note 1: ABSIO: The end coordinate system of the end of previous block in workpiece coordinate system.
Note 2: ABSMT: The current machine tool coordinate system position in its system.
Note 3: ABSOT: The current coordinate position in workpiece coordinate system.
Note 4: ABSKP: The skip signal in G31 block is with the enabled position in workpiece coordinate system.
VOLUME I
PROGRAMMING
3) Zero offset values of workpiece and addition:
Table 4-9-2-4
Variable
Function
No.
#5201
…
External workpiece zero point offset value along the 1st axis
…
#5204
External workpiece zero point offset value along the 4th axis
#5206
G54 workpiece zero offset value along the 1st axis
…
…
#5209
G54 workpiece zero offset value along the 4th axis
#5211
G55 workpiece zero offset value along the 1st axis
…
…
#5214
G55 workpiece zero offset value along the 4th axis
#5216
G56 workpiece zero offset value along the 1st axis
…
…
#5219
G56 workpiece zero offset value along the 4th axis
#5221
G57 workpiece zero offset value along the 1st axis
…
…
#5224
G57 workpiece zero offset value along the 4th axis
#5226
G58 workpiece zero offset value along the 1st axis
…
…
#5229
G58 workpiece zero offset value along the 4th axis
#5231
G59 workpiece zero offset value along the 1st axis
…
…
#5234
G59 workpiece zero offset value along the 4th axis
#7001
G54 P1 workpiece zero offset value along the 1st axis
…
…
153
GSK218MC Series Machining CNC System
Programming & Operation Manual
#7004
G54 P1 workpiece zero offset value along the 4th axis
#7006
G54 P2 workpiece zero offset value along the 1st axis
…
…
#7009
G54 P2 workpiece zero offset value along the 4th axis
#7246
G54 P50 workpiece zero offset value along the 1st axis
…
…
G54 P50 workpiece zero offset value along the 4th axis
#7249
4. Local variable
The corresponding relationships between addresses and local variables are shown below:
Table 4-9-2-5
VOLUME I
PROGRAMMING
Argument
Local variable
Add.
No.
A
Argument Add.
Local variable No.
#1
Q
#17
B
#2
R
#18
C
#3
S
#19
I
#4
T
#20
J
#5
U
#21
K
#6
V
#22
D
#7
W
#23
E
#8
X
#24
F
#9
Y
#25
M
#13
Z
#26
Note 1: The assignment is performed by that the English letter adds the numerical value, the rest of 20 letters can be
assigned to argument other than the G, L, O, N, H and P. Each letter only can be assigned once, from
A-B-C-D… to X－Y－Z, and the assignment can be performed regardless of the alphabet sequence, and the
addresses without assignment can be omitted.
Note 2: There is not alternative other than to specify the G65 before using any argument.
5. The precautions about the user macro program body
1) Input by keyboard
Press the # followed with the parameter words G, X, Y, Z, R, I, J, K, F, H, M, S, T, P and Q, and
then the # is inputted.
2) The calculation can be commaned and the code can be shifted in MDI state.
3) The H, P, Q and R of the calculation and shifting codes are regarded as the parameter
specified by G65 whenever before or after G65.
154
H02 G65 P#100 Q#101 R#102 ;
Correct
N100 G65 H01 P#100 Q10 ;
Correct
Chapter Four Preparatory Function G Code
4) The input range of variable can not be exceeded the available 15-digit; its calculation results
should be less than 9 integer digits; the manual input range of variable are the enabled 8-digit.
5) The calculation result of variable can be performed by decimal, and its accuracy is 0.0001.
The rest of calculations will not discard the decimal other than the H11 (OR calculation), H12
(AND calculation), H13 (NON calculation) and H23 (Remainder calculation) may omit the
decimal in variable during calculating.
For example:
#100 ＝ 35, #101 ＝ 10,
#102 ＝ 5
(＝3.5)
#111 ＝ #110×#102
(＝17.5)
#120 ＝ #100×#102
(＝175)
#121 ＝ #120÷#101
(＝17.5)
6) The performance time of calculation and shifting codes are variable according to the
conditions; generally, the average value can be considered as 10ms.
7) When the variable does not define, the variable may become “Null”. Variable #0 is always null,
which can be wrote only instead of reading.
a. Quotation
When an undefined variable is quoted, the address, itself, is also ignored.
For example:
When the variable #1 is 0, and the variable #2 is null, the performance result of G00X#1
Y#2 is G00X0;
b. Operation
<Vacant> is the same as 0 except when evaluating by <vacant>.
Table 4-9-2-6
When #1=<vacant>
When #1=0
#2=#1
#2=#1
↓
↓
#2=<vacant>
#2=0
#2=#1*5
#2=#1*5
↓
↓
#2=0
#2=0
#2=#1+#1
#2=#1+#1
↓
↓
#2=0
#2=0
c. Conditional expressions
<Vacant> deffers from 0 only for EQ and NE.
155
VOLUME I
PROGRAMMING
#110 ＝ #100÷#101
GSK218MC Series Machining CNC System
Programming & Operation Manual
Table 4-9-2-7
When #1=<vacant>
When #1=0
VOLUME I
PROGRAMMING
#1 EQ #0
#1 EQ #0
↓
↓
Established
Not established
#1 NE #0
#1 NE #0
↓
↓
Not established
Established
#1 GE #0
#1 GE #0
↓
↓
Established
Established
#1 GT #0
#1 GT #0
↓
↓
Not established
Not established
Fig. 4-9-2-2
When the value of a variable is blank, the variable is null.
156
Chapter Four Preparatory Function G Code
4.9.3
User Macro Program Call
When G65 is specified, the user macro program specified at address P is called, and the data
can be passed to the custom macro program by argument.
Format:
G65 P □□□□□L□□□□ <Argument specification>；
Numbers of calling
The program number of called macro program body
The program number of user macro program can be specified by address P followed with G65. L
Specify the repeated times from 1 to 9999 after address L when a number of repititions are
required. 1 is assumed when L is omitted.
By using argument specification, values are assigned to corresponding local variables.
Note 1: When the subprogram number specified by address P can not be indexed, an alarm (PS 078) occurs.
Note 2: The subprograms from No. 90000~9999 is the reserved program by system, when user calls this subprogram,
the system can execute the conent of the subprogram; however, the cursor may always stop at the G65 code
section, and the main program content will always show on the program interface. (The content of subprogram
can be displayed by modifying the bit 4 of parameter No.: 27.
Note 3: Never attempt to call the macro program in DNC mode.
Note 4: Up to 5-layer can be nested for the macro program calling.
4.9.4
User Macro Program Function A
1. Common form:
G65 Hm P#i Q#j R#k ;
m: 01～99 means the function of operation code or the shifting code.
#i: The variable name for registering the operation result
#j: The variable name 1 for operating. It also can be regarded as constant; and the constant can
be expressed directly regardless of the #.
#k: The variable name 2 for operating. It also can be treated as constant.
Meaning:
#i = #j ○ #k
└─────── Operation symbol, it is specified by Hm.
(For example) P#100 Q#101 R#102……#100 = #101 ○ #102 ;
P#100 Q#101 R15 ……#100 = #101 ○ 15 ;
P#100 Q-100 R#102……#100 = -100 ○ #102
The H code specified by G65 is without any effect for selecting the offset value.
157
VOLUME I
PROGRAMMING
specifies the call times of macro program; and the argument passes the data to macro program.
GSK218MC Series Machining CNC System
G code H code
Function
Programming & Operation Manual
Defintion
#i ＝ #j
#i ＝ #j + #k
VOLUME I
PROGRAMMING
G65
H01
Assignment
G65
H02
Plus
G65
G65
H03
G65
H04
H05
Minus
Multiplication
Division
G65
H11
Logic plus (OR)
G65
H12
Logic multiplication
(AND)
#i ＝ #j OR #k
#i ＝ #j AND #k
G65
H13
Exclusive OR
#i ＝ #j XOR #k
G65
H21
Square root
G65
H22
Absolute
#i ＝ #j
#i ＝ #j
G65
H23
Remainders
#i＝#j-trunc(#j ÷ #k)×#k
G65
G65
G65
G65
G65
G65
G65
G65
G65
G65
G65
G65
G65
G65
H26
H27
H31
H32
H33
H34
H80
H81
H82
H83
H84
H85
H86
H99
#i ＝ #j - #k
#i ＝ #j × #k
#i ＝ #j ÷ #k
Complex multiplication &
division operations
#i ＝ (#i × #j) ÷ #k
Complex square root #i ＝ #j2+#k2
Sine
#i ＝ #j×SIN(#k)
#i ＝ #j×COS(#k)
Cosine
Tangent
#i ＝ #j×TAN(#k)
Arc tangent
#i ＝ ATAN(#j/#k)
Unconditional branch Turn to N
Conditional branch 1 IF #j ＝ #k， GOTO N
Conditional branch 2 IF #j ＝ #k， GOTO N
Conditional branch 3 IF #j ＞ #k， GOTO N
Conditional branch 4 IF #j ＜ #k， GOTO N
Conditional branch 5 IF #j ＞ #k， GOTO N
Conditional branch 6 IF #j ＜ #k， GOTO N
Alarm
Fig. 4-9-4-1
2. Operation code:
1) The assignment of variable: # I = # J
G65 H01 P#I Q#J；
158
(For example) G65 H01 P#101 Q1005；
（#101 = 1005）
G65 H01 P#101 Q#110；
（#101 = #110）
G65 H01 P#101 Q-#102；
（#101 = -#102）
Chapter Four Preparatory Function G Code
2) Plus operation: # I = # J+# K
G65 H02 P#I Q#J R#K；
(For example) G65 H02 P#101 Q#102 R15；
（#101 = #102+15）
3) Minus operation: # I = # J- #K
G65 H03 P#I Q#J R# K；
(For example) G65 H03 P#101 Q#102 R#103；
（#101 = #102-#103）
4) Multiplication operation: # I = # J×# K
G65 H04 P#I Q#J R#K；
(For example) G65 H04 P#101 Q#102 R#103；
（#101 = #102×#103）
VOLUME I
PROGRAMMING
5) Division operation: # I = # J÷# K
G65 H05 P#I Q#J R#K；
（#101 = #102÷#103）
(For example) G65 H05 P#101 Q#102 R#103；
6) Logic plus (OR): # I = # J.OR. # K
G65 H11 P#I Q#J R#K；
(For example) G65 H11 P#101 Q#102 R#103；
（#101 = #102.OR. #103）
7) Logic multiplication (AND): # I = # J.AND. # K
G65 H12 P#I Q#J R#K；
(For example) G65 H12 P# 101 Q#102 R#103；
（#101 = #102.AND.#103）
8) XOR: # I = # J.XOR. # K
G65 H13 P#I Q#J R#K；
(For example) G65 H13 P#101 Q#102 R#103；
（#101 = #102.XOR. #103）
9) Square root：# I =
#j
G65 H21 P#I Q#J；
(For example) G65 H21 P#101 Q#102 ;
（#101=
#102 ）
10) Absolute: # I = | # J |
G65 H22 P#I Q#J ；
(For example) G65 H22 P#101 Q#102 ；
（#101 = | #102 |）
11) Remainder: # I = # J－TRUNC(#J/#K)×# K, TRUNC: Reject the decimal section
G65 H23 P#I Q#J R#K；
(For example) G65 H23 P#101 Q#102 R#103； （#101 = #102- TRUNC (#102/#103)×#103）
12) Complex devision operation: # I =（# I×# J）÷# K
G65 H26 P#I Q#J R# k；
(For example) G65 H26 P#101 Q#102 R#103；
（#101 =（#101×# 102）÷#103）
159
GSK218MC Series Machining CNC System
Programming & Operation Manual
2
13) Complex square root I = #j +#k2
G65 H27 P#I Q#J R#K；
(For example) G65 H27 P#101 Q#102 R#103； (#101 =
#1022+ #1032 )
14) Sine: # I = # J•SIN (# K) (Unit：°)
G65 H31 P#I Q#J R#K；
(For example) G65 H31 P#101 Q#102 R#103；
（#101 = #102•SIN（#103））
15) Cosine: # I = # J•COS (# K) (Unit：°)
G65 H32 P#I Q#J R# K；
(For example) G65 H32 P#101 Q#102 R#103；
（#101 =#102•COS（#103））
VOLUME I
PROGRAMMING
16) Tangent: # I = # J•TAN (# K) (Unit：°)
G65 H33 P#I Q#J R# K；
(For example) G65 H33 P#101 Q#102 R#103；
（#101 = #102•TAN（#103））
17) Arc tangent: # I = ATAN (# K) (Unit：°)
G65 H34 P#I Q#J R# K；
(For example) G65 H34 P#101 Q#102 R#103；
（#101 =ATAN（#102/#103））
Note 1: The unit of angle variable is degree.
Note 2: In each operation, when the necessary Q and R are not specified, its value regards as zero to operate.
Note 3: trunc: Rounding operation, eject the decimal section.
3. Branch command
1) Unconditional branch
G65 H80 Pn；
n：Sequence number
(For example) G65 H80 P120;
(Trun to N120 block)
2) Conditional branch 1 #J.EQ.# K (＝)
G65 H81 Pn Q#J R# K；
n：Sequence number
(For example) G65 H81 P1000 Q#101 R#102；
When # 101 = #102, turn to N1000 block, when #101 ≠ #102, program performes with
sequentially.
3) Conditional branch 2 #J.NE.# K (≠)
G65 H82 Pn Q#J R# K；
n：Sequence number
(For example) G65 H82 P1000 Q#101 R#102；
When # 101 ≠ #102, turn to N1000 block, when #101 = #102, program performs with
sequentially.
4) Conditional branch 3 #J.GT.# K (＞)
160
Chapter Four Preparatory Function G Code
G65 H83 Pn Q#J R# K；
n：Sequence number
(For example) G65 H83 P1000 Q#101 R#102；
When #101 ＞ #102, turn to N1000 block, when #101 ≤ #102, program performs with
sequentially.
5) Conditional branch 4 #J.LT.# K (＜)
G65 H84 Pn Q#J R# K；
(For example)
n：Sequence number
G65 H84 P1000 Q#101 R#102；
When # 101 ＜ #102, turn to N1000 block, when #101 ≥ #102, program performs with
sequentially.
6) Conditional branch 5 #J.GE.# K (≥)
(For example)
n：Sequence number
G65 H85 P1000 Q#101 R#102；
When # 101 ≥ #102, turn to N1000 block, when #101 ＜ #102, program performs with
sequentially.
7) Conditional branch 6 #J.LE. # K (≤ )
G65 H86 Pn Q#J R# K；
n：Sequence number
(For example) G65 H86 P1000 Q#101 R#102；
When # 101≤ #102, turn to N1000 block, when #101 ＞ #102, program performs with
sequentially.
Note: The sequence number can be specified by variable. For example: G65 H81 P#100 Q#101 R#102; the
program moves to the block specified by #100 sequence number when the condition is executed.
4. Logic AND, OR and NON codes
For example:
G65 H01 P#101 Q3；
G65 H01 P#102 Q5；
G65 H11 P#100 Q#101 Q#102；
5 means that the binary is 101, 3 means 011, the calculation result is #100=7;
G65 H12 P#100 Q#101 Q#102；
5 means that the binary is 101, 3 means 011, the calculation result is #100=1;
5. Macro variable alarm
For example:
G65 H99 P1；
Macro variable 3001 alarms
G65 H99 P124；
Macro variable 3124alarms
161
VOLUME I
PROGRAMMING
G65 H85 Pn Q#J R# K；
GSK218MC Series Machining CNC System
Programming & Operation Manual
The example of user macro program
1. Bolt hole cycle
The center is regarded as reference position (X0, Y0), radius is (R), and start angle is (A); N
holes can be machined accordingly.
Y
The 3rd hole
The 2nd hole
The 1st hole
R
VOLUME I
PROGRAMMING
Reference
position
(X0,Y0)
The Nth hole
A
The (N-1)th
hole
X
Fig. 4-9-4-2
X0, Y0 are the reference point coordinate value of the bolt hole cycle.
R: Radiu, A: Start angle, N: Numbers. The above-mentioned parameters are used the following
variables.
#500: The coordinate value (X0) of reference position X
#501: The coordinate value (Y0) of reference position Y
#502: Radius (R)
#503: Start angle (A)
#504: N numbers
N＞0, CCW, numbers N.
N＜0, CW, numbers N.
The following variables are used the operation in the macro program.
#100: The 1st hole machining counting (I)
#101: Terminal value of counting (＝┃N┃) (IE)
#102: The angle (θI) of the 1st hole
#103: The X coordinate value (Xi) of the 1st hole
#104: The Ycoordinate value (Yi) of the 1st hole
The user macro program body can be written as the following forms:
O9010；
N100 G65 H01 P#100 Q0；
I＝0
G65 H22 P#101 Q#504；
IE＝|N|
N200 G65 H04 P#102 Q#100 R360；
162
Chapter Four Preparatory Function G Code
G65 H05 P#102 Q#102 R#504；
θI＝A＋360°×I/N
G65 H02 P#102 Q#503 R#102；
G65 H32 P#103 Q#502 R#102；
X I＝X I＋R·COS(θI)
G65 H02 P#103 Q#500 R#103；
G65 H31 P#104 Q#502 R#102；
Y I＝Y I＋R·SIN(θI)
G65 H02 P#104 Q#501 R#104；
G90 G00 X#103 Y#104；
The 1st hole positioning
G**；
The concrete hole machining G code
G65 H02 P#100 Q#100 R1；
I＝I＋1
G65 H84 P200 Q#100 R#101；
When I＜IE, turn to N200 to machin the hole of
VOLUME I
PROGRAMMING
IE
M99；
Call the program examples of the above-mentioned user macro program body:
O0010；
G65 H01 P#500 Q100；
X0=100MM
G65 H01 P#501 Q-200； Y0=-200MM
G65 H01 P#502 Q100；
R=100MM
G65 H01 P#503 Q20；
A=20°
G65 H01 P#504 Q12；
N=12 CCW
G92 X0 Y0 Z0；
M98 P9010；
User macro program calling
G80；
X0 Y0；
M30；
4.9.5
User Macro Program Function B
1. Arithmetic and Logic operation
The operations listed in the following table can be performed on variables. The expression at the
right of the operator can contain constants and/or variables combined by a function or operator.
Variable #j and #k in an expression can be replaced with a constant. Variable at the left can also be
assigned with an expression.
163
GSK218MC Series Machining CNC System
Table 4-9-5-1
Programming & Operation Manual
Arithmetic and logic operation
Format
Definition
#i = #j
Sum
#i = #j + #k;
Difference
#i = #j - #k;
Product
#i = #j * #k;
Quotient
#i = #j / #k;
Sine
#i = SIN[#j];
Arcsine
#i = ASIN[#j];
Cosine
#i = COS[#j];
Arccosine
#i = ACOS[#j];
Tangent
#i = TAN[#j];
Arctangent
#i = ATAN[#j] / [#k];
Square root
#i = SQRT[#j];
Absolute value
#i = ABS[#j];
Rounding off
#i = ROUND[#j];
Rounding up
#i = FUP[#j];
Rounding down
#i = FIX [#j];
Nature logarithm
#i = LN[#j];
Exponential
#i = EXP[#j];
VOLUME I
PROGRAMMING
Function
Remark
An angle is specified in
degree. 90°30’ means
90.5 degrees.
function
OR
#i = #j OR #k;
A logic operation is
XOR
#i = #j XOR #k;
performed based on
AND
#i = #j AND #k;
binary numbers bit by bit.
Conversion from
#i = BIN[#j];
BCD to BIN
Conversion from
It used to the signal
#i = BCD[#j];
exchange for PMC.
BIN to BCD
Explanations:
(1) Angle unit
The units of angles used with the SIN, COS, ASIN, ACOS, TAN and ATAN functions are
degrees. For example, 90°30’ is represented as 90.5 degrees.
（2）ARCSIN
(2) ARCSIN
#i = ASIN [ #j ]
#i = ASIN [ #j ]
Solution ranges from -90°～90°.
When #j is beyond the range of -1 to 1, system alarm is issued.
164
Chapter Four Preparatory Function G Code
A constant can be used instead of the #j variable.
（3）ARCCOS
(3) ARCCOS
#i = ACOS [ #j ]
#i = ACOS [ #j ]
The solution ranges from 180° to 0°.
When #j execeeds the range of -1 to 1, system alarm is generated.
A constant can be used instead of the #j variable.
（4）ARCTAN
(4) ARCTAN
#i = ATAN [ #j ] / [ #k ]
#i = ATAN [ #j ] / [ #k ]
Specify the length of two sides, separated by a slahs (/).
VOLUME I
PROGRAMMING
The solution range from 0° to 360°.
[For example] When #1 = ATAN [ -1 ] / [ -1 ]; is specified, #1=225°.
A constant can be replaced by # j variable.
(5) Nature logarithm
#i = LN [ #j ]
When the antilogarithm (# j) is zero or smaller, the system alarm occurs.
A constant can be replaced by # j variable.
(6) Exponential function
#i = EXP [ #j ]
When the result of operation exceeds 99997.453535 (#j is about 11.5129), an overflow
occurs and the system alarm issues.
A constant can be replaced by # j variable.
(7) ROUND function
ROUND function rounds off at the 1st decimale position.
For example:
When #1=ROUND[#2]; is executed where #2=1.2345, the value of variable 1 is 1.0.
(8) Round down and round up
With CNC, when the absolute value of the integer produced by an operation on a number is
greater than the absolute value of the original number, such an operation is referred to as
rounding up to an integer. Conversely, when the absolute value of the integer produced by an
operation on a number is less than the absolute value of the original number, such an operation
is referred to as rounding down to an integer. Be particularly careful when handing negative
numbers.
Examples:
Suppose that #1=1.2, #2=－1.2。
When #3=FUP[#1] is executed, 2.0 is assigned to #3.
When #3=FIX[#1] is executed, 1.0 is assigned to #3。
165
GSK218MC Series Machining CNC System
Programming & Operation Manual
When #3=FUP[#2] is executed, －2.0 is assigned to #3。
When #3=FIX[#2] is executed, －1.0 is assigned to #3。
(9) Abbreviations of arithmetic and logic operation commands
When a function is specified in a program, the first two characters of the function name can
be used to specify the function. (See the table 4-9-5-1).
Example:
ROUND→RO
FIX→FI
(10) Priority of operations
VOLUME I
PROGRAMMING
① Function
② Operations such as multiplication and devision (* / AND)
③ Operations such as addition and subtraction (+ - OR XOR)
Example) #1 = #2 + #3 * SIN[#4] ;
1
2
3
1 ,
2 and 3 indicate the order of operations.
(11) Restriction
[, ] uses the enclosed expressions.
When specifying the divisor 0 or TAN[90] in division operation, system alarm is then
issued.
2. Branch and Repetition
1) Branch and Repetition
In a program, the flow of control can be changed using the GOTO statement and IF statement.
Three types of branch and repetition operations are used:
Branch and
repetition
GOTO statement (Unconditional branch)
IF statement (Conditional branch:
IF…THEN…)
WHILE statement (Repetition while…)
2) Unconditional branch
¾
GOTO statement
Branch to the block marked with sequence number n. A sequence number can also be specified
using an expression.
166
Chapter Four Preparatory Function G Code
GOTOn;
n: Sequence number (1 to 99999）
Example:
GOTO 1；
GOTO #10；
3) Conditional branch (IF statement) [<Conditional expression>]
IF[<Conditional expression >]GOTO n
If the specified conditional expression is satisfied, Branch to the block marked with sequence
number n. If the specified conditional expression is not satisfied, the next block is executed.
If the condition is
not satisfied
VOLUME I
PROGRAMMING
If the variable value #1 is greater than 10, branch to the block with
sequence number N2.
IF [#1 GT 10] GOTO 2 ;
If the condition is
saftisfied
Program
N2 G00 G91 X10.0 ;
:
IF[<Conditional expression>]THEN
If the conditional expression is satisfied, a predetermined macro program statement is executed.
Only a single macro statement is carried out.
If the value of #1 and #2 are the same, 0 is assigned to #3.
IF[#1 EQ #2] THEN #3=0;
Explanations:
¾
Conditional expression
A conditional expression must include an operator inserted between two variables or between a
variable and constant, and must be enclosed in brackets ([, ]). An expression can be replaced a
variable.
¾
Operators
Operators consist of two letters and used to compare two values to determine whether they are
equal or one value is smaller or greater than the other one.
Table 4-9-5-2
Operators
Operator
Meaning
EQ
Equal to（=）
NE
Note equal to（≠）
GT
Greater than（>）
167
GSK218MC Series Machining CNC System
¾
Programming & Operation Manual
GE
Greater than or equal to（≥）
LT
Less than（<）
LE
Less than or equal to（≤）
Typical program
The sample program below finds the total of numbers 1 to 10.
VOLUME I
PROGRAMMING
O9500；
#1=0；
#2=1；
N1 IF[#2 GT 10]GOTO 2;
#1=#1+#2；
#2=#2+1；
GOTO 1；
N2 M30；
Initial value of the variable to hold the sum
Initial value of the variable as an addend
Branch to N2 when the addend is greater than 10
Calculation to find the sum
Next addend
Branch to N1
End of program
4) Repetition (WHILE statement)
Specify a conditional expression after WHILE. While the specified consition is satisfied, the
program from DO to END is executed; otherwise, turn to the block after END.
If the condition is
not satisfied
WHILE[Conditional expression] DO m;
(m=1,2,3)
If the condition
is satisfied
Program
END m ;
:
When the specified condition is satisfied, the program from DO to END after WHILE is executed;
otherwise, it may perform the block after END. This kind of command format is suitable for the IF
statement. The numbers followed with the DO and END are specified the labels of the program
execution range. The numbers 1, 2 and 3 can be used. When a number other than 1, 2, and 3 is used,
the alarm may occur.
Explanation:
¾
Nesting
The identification numbers (1 to 3) in a DO——END cycle can be used as many times as desired.
Note, when a program includes the overlapping of the crossing repetition cycle DO ranges, the alarm
may issue.
168
Chapter Four Preparatory Function G Code
1. Numbers (1 to 3) can be used
as many times as required.
WHILE[ … ] DO 1;
Program
3. DO cycle can be nested to a Max.
depth of 3 levels.
WHILE[ … ] DO 1;
：
WHILE[ … ] DO 2;
：
WHILE[ … ] DO 3;
END 1 ;
:
Program
WHILE[ … ] DO 1;
END 3 ;
Program
VOLUME I
PROGRAMMING
END 2 ;
END 1 ;
:
2. The range of DO can not be crossed
WHILE[ … ] DO 1;
Program
WHILE[ … ] DO 2;
:
END 1 ;
END 1 ;
4. Control can be transferred to the
outside of a repetition.
WHILE[ … ] DO 1;
IF[…] GOTO n ;
END 1 ;
Nn
Program
END 2 ;
Explanations：
¾
Infinite cycle
When DO is specified instead of specifying the WHILE statement, an infinite cycle ranging from
DO to END is produced.
¾
Processing time
When the GOTO statement marked with a branch is treated, and the sequence number index is
performed. For this reason, the processing in the reverse direction takes a longer time than
processing in the forward direction. Using the WHILE statement for repetition reduces processing
time.
¾
Undefined variable
In the condtional expression that uses EQ or NE, a <vacant> and zero have different effects. In
169
GSK218MC Series Machining CNC System
Programming & Operation Manual
other types of conditional expressions, a <vacant> is regarded as zero.
¾
Typical program
The sample program below counts the total of numbers 1 to 10.
O0001 ；
#1=0；
#2=1；
WHILE [#2 LE 10] DO 1;
#1=#1+#2;
#2=#2+1;
END 1;
M30;
VOLUME I
PROGRAMMING
Precautions:
z
When a macro program is called by G65 and a variable is quoted by F, the system performs
based upon the variable value.
z
Do not use the cycle and skip command in DNC.
z
GOTO statement searches downward from the current block; if it can not find the corresponding
sequence number and then research again back to the beginning of the program. Do not use the
identical N codes in a same program as much as possible.
z
When the decimal means the variable number, the system will directly discard the decimal
section instead of considering the carry-bit
z
The value of the local variable will always hold before the end of main program, which is used
together within each subprogram.
170
Chapter Five
CHAPTER FIVE
Miscellance Function M Code
MISCELLANEOUS FUNCTION M CODE
The M codes for this machine tool can be used by user, which shows below:
Table 5-1
M code
M30
M code for
Program ends and turns to the beginning of the program,
maching number adds 1.
Program ends and turns to the beginning of the program,
maching number adds 1.
M98
Subprogram calling
M99
Sbuprogram ends and returns/repeatedly perform
M00
Program dwell
M01
Program dwell selection
PLC controls the
M03
Spindle positive
M code
M04
Spindle reverse
M05
Spindle stop
M06
Tool-change
M08
Cooling ON
M09
Cooling OFF
M10
A axis releasing
M11
A axis clamping
M16
Tool control releasing
M17
Tool control clamping
M18
Spindle orientation cancellation
M19
Spindle orientation
M20
Spindle neutral command
M21
Cutter-search code in tool return
M22
Cutter-search code in capturing a new tool
M26
Punching water-valve ON
M27
Punching water-valve OFF
M28
Cancel the rigid tapping
M29
Rigid tapping command
M35
Start the chip-removal promotion conveyor
M36
Close the chip-removal promotion conveyor
M44
Start the spindle blowing
program
VOLUME I
PROGRAMMING
controlling the
M02
Function
171
GSK218MC Series Machining CNC System
Programming & Operation Manual
M45
Close the spindle blowing
M50
Start the automation tool-change
M51
Close the automation tool-change
The movement code and the miscellaneous function are simultaneously performed when they
are shared with a same block.
When the numerical value followed with the address M is specified, the code signal and strobe
signal are conveyed to the machine tool to switch on or off this functions using machine. Usaully, only
one M code can be specified in one block. Up to 3 M codes in one block can be specified by setting
the bit 7 of parameter No.: 33. However, some M codes can not be specified at the same time due to
mechanical operation restrictions. For detailed information about the mechanical operation
VOLUME I
PROGRAMMING
restrictions on simultaneous specification of multiple M codes in one block, refer to the manual of
each machine tool builder.
5.1
M Code Control by PLC
A M code and a movement code are simultaneously performed when the M code controlled by
PLC shares the same block with a movement code.
5.1.1
Negative/Reverse Code Command (M03, M04)
Code: M03 (M04) Sx x x;
Explanation: The positive rotation is observed from negative to position along with the Z axis,
spindle CCW is regarded as positive; and CW is treated as reverse. Entering the rotation
direction of workpiece based upon the right helix is regarded as positive, and the leaving the
rotation direction of workpiece based upon the right helix is treated as reverse.
Sx x x code, is the spindle speed, is the located gear when the gear is controlled.
Unit: rev./min/ (r/min)
Sx x x is the actual speed when the frequency conversion is controlled. For example: S1000
specifies that the spindle is revolved based upon the 1000r/min.
5.1.2
Spindle Stopping Code Command M05
Code: M05, spindle will stop rotating when performing M05 in Auto method. However, the
commanded speed by S code is reserved. The deceleration method in spindle stop is
determined by the machine tool manufacturer. Generally, it is the energy-consumption brake.
172
Chapter Five
5.1.3
Miscellance Function M Code
Cooling ON/OFF (M08, M09)
Code: M08, control the ON of the cooling water pump. M09, control the OFF of the cooling water
pump. In the Auto mode, the water pump control code does not execute if the miscellaneous
function locking is performed.
5.1.4
A Axis Releasing/Clamping (M10, M11)
Code: M10, A axis releasing. M11, A axis clamping
VOLUME I
PROGRAMMING
5.1.5
Tool Control Tool-releasing/Tool Clamping (M16, M17)
Code: M16, tool-releasing control. M17, tool-clamping control
5.1.6
Spindle Orientation/Cancellation (M18, M19)
Code: M18, spindle orientation cancels. M19, spindle orients for using the tool-change positioning.
5.1.7
Tool-searching Code Command (M21, M22)
Code: M21, the tool-searching code in cutter-return; M22, the tool-searching code in capturing a new
tool.
5.1.8
Tool-magazine Return Code Command (M23, M24)
Code: M23, tool-magazine swings to the code of spindle position; M24, tool-magazine swings to
code of original position.
5.1.9
Rigid Tapping (M28, M29)
Code: M28, cancel the rigid tapping. M29, rigid tapping.
173
GSK218MC Series Machining CNC System
5.1.10
Programming & Operation Manual
Helical Chip-removal Conveyor ON/OFF (M35, M36)
Code: M35, control the start of the helical chip-removal conveyor. M36, control the stop of the helical
chip-removal conveyor.
5.1.11 Punching Water Valve ON/OFF (M26, M27)
Code: M26 is puncing water valve ON; M27 is puncing water valve OFF.
VOLUME I
PROGRAMMING
5.1.12
Spindle Blowing ON/OFF (M44, M45)
Code: M44, Spindle blowing contron ON. M45, Spindle blowing contron OFF.
5.1.13
Automatic Tool-change Start/End (M50, M51)
Code: M50, Start the automatic tool-change control. M51, End the automatic tool-change control.
5.2
M Codes for Controlling Program
The M codes for controlling the program are divided into main program control and macro
program control. Firstly perform the movement code, and then perform the M code when the M codes
for controlling program are shared the same block with the movement code.
Notice: 1. M00, M01, M02, M06, M30, M98 and M99 codes can not be specified together with other M codes;
otherwise, the system alarm occurs. When the above-mentioned M codes are shared the same block with
other codes (except the M codes), the other codes in the same block will firstly perform and then perform
these M codes.
2. These M codes include that the CNC conveys the M codes to the machine tool, simultaneously, the CNC can
also performs the internal operation code; for example, the M code for the program prereading function is
disabled. Additional, the CNC conveys only the M code to machine tool instead of executing the M code of
the internal operation, which can be specified within the same block.
5.2.1
Program End and Return (M30, M02)
In the Auto operation, program stops the automatic state when operating to M30 (M20), the
followed program will not perform and the spindle and cooling operation will stopped according; the
workpiece machining number adds 1. M30 can be controlled whether it returns to the beginning of
174
Chapter Five
Miscellance Function M Code
program by bit 4 of No.: 33; M02 can be controlled whether it returns to the beginning of program by
bit 2 of No.: 33. If the M02 and M30 are performed at the end of the subprogram, return to program of
the subprogram calling, and then continue perform the following blocks.
5.2.2
Program Dwell (M00)
In the Auto mode, the automatic state dwells when program operates to the M00. In this case,
the previous modal information will registered and it continues by the repeated start button. The
function equals to the feed hold button by pressing.
Program Optional Dwell (M01)
In the Auto mode, the optional dwell automatic operating state when program moves to the M01;
if the “Optional stop” switch is turned on, the M01 shares same effect with M00; if the “Optional stop”
switch is turned off, regardless of the M01 code. Refer to the Operation Manual for details.
5.2.4
Program Calls Subprogram Code Command (M98)
M98 code can be compiled in main program to call the performance of subprogram. Refer to the
following format:
M98 P
L
Repeated calling times
The called subprogram
series number
Fig. 5-2-4-1
5.2.5
Program Ends and Rturns (M99)
1. In the Auto mode, if a M99 uses at the end of the main program, which returns to the beginning
of the program to automatically perform when the program operates to M99; the following
programs will not execute, and the workpiece machining number does not accumulate.
2. Using M99 at the end of subprogram, the program will return to main program after operting
this block, and then continue executing by calling the next program of the subprogram.
3. M30 is treated by M99 in the DNC mode, and the cursor stops at the end of the program.
175
VOLUME I
PROGRAMMING
5.2.3
GSK218MC Series Machining CNC System
VOLUME I
PROGRAMMING
176
Programming & Operation Manual
Chapter Six Spindle Function S Code
CHAPTER SIX
SPINDLE FUNCTION S CODE
The code signal conveys to machine tool after converting into analog signal by the S codes and
its following numerical values, which is used for the spindle control of the machine tool. S is regarded
as modal value.
6.1
Spindle Analog Control
When the SPT of the bit 2 of parameter No.: 1 sets to 0, the address S and its following
for details.
Code format: S_
Explanations:
1. One S code can be specified in a block.
2. The spindle can be directly specified by the address S and its following data, its unit is
rev./min (r/min). For example: M3 S300 means that the spindle operates based upon the
300 rev./min.
3. When the movement code and S code are shared with a same block, which are
performed simultaneously.
4. The spindle can be controlled by the S code and its following numerical values.
6.2
Spindle Switch Value Control
When the SPT of the bit 2 of parameter No.: 1 sets to 1, the spindle speed can be controlled by
the address S and its following 2-digit switch value.
When the spindle speed is controlled by selecting a switch value, the system then can offers
3-level spindle mechanical gear-shifting. Refer to the manual made by the manufacturer for the
corresponding relationships and the spindle shifing levels provide by machine tool of S code and
spindle speed.
Code format: S01 (S1) ;
S02 (S2) ;
S03 (S3) ;
Explanations:
1. At present, there are 8 shiftings for the software, but the ladder diagram is only 3. When
the above-mentioned codes other than the S codes are specified, the system then
displays the “The miscellaneous function is being performed…”.
177
VOLUME I
PROGRAMMING
numerical value can be controlled the spindle speed byanalog voltage; refer to the operation manual
GSK218MC Series Machining CNC System
Programming & Operation Manual
2. If the 4-digit followed with S are specified, the later 2-digit are then enabled.
6.3
Constant Surface Cutting Speed Control (G96/G97)
Code format:
Constant surface speed control code
G96 S_
Constant surface speed control code cancellation
Constant surface speed controlled axis code
Surface speed (mm/min or inch/min)
G97 S_
G96 P_
Spindle speed (r/min)
P1 X axis; P2 Y axis; P3 Z axis;
th
P4 the 4 axis
Clamp of Max. spindle speed
G92 S_
S specifies the Max. spindle speed (r/min)
VOLUME I
PROGRAMMING
Function: Specify the surface speed (relative speed between the tool and workpiece) following S.
The spindle is rotated so that the surface speed is constant regardless of the tool position.
Explanations:
1. G96 is a modal code. After a G96 command is specified, the program enters the constant
surface speed control mode, and the S value is regarded as surface speed.
2. A G96 code must specify the axis along with constant surface speed control is applied. A G97
code cancels the G96 mode.
3. It is necessary to set a workpiece coordinate system for performing the constant surface
cutting feed control, so that the center coordinate of rotation axis changes into zero.
X
0
Z
Fig. 6-3-1 The controlled workpiece coordinate system of constant surface cutting speed
4. When constant surface speed control is applied, a spindle speed higher than the value
specified in G92 S_, it is convenient to clamp at the Max. spindle speed. When the power is
turned on, the Max. spindle speed is not yet set. The S is regarded as S=0 in a G96 code till
M3 or M4 appears in program.
178
Chapter Six Spindle Function S Code
Spindle speed (rpm)
n
The spindle speed
almost coincides with
the surface speed at
approx.160mm (radius).
3000
2800
2600
2400
2200
2000
1800
1600
1400
VOLUME I
PROGRAMMING
1200
Surface speed S
is 600mm/min
1000
800
600
400
200
Radius (mm)
0
0 20 40 60 80 100120 140 160180 200 220240 260 280 300
Fig. 6-3-2
Relationships among the workpiece radius, spindle speed and surface speed
5. Specify surface cutting feed in G96 mode:
179
GSK218MC Series Machining CNC System
G96 mode
Programming & Operation Manual
G97 mode
Specify surface speed in
mm/min (inch/min)
G97
command
Store this speed in
mm/min (inch/min)
VOLUME I
PROGRAMMING
Specified
Specify
the
spindle
speed
Apply the
specified spindle
speed (rpm)
Without
specification
Surface speed (mm/min or
inch/min) converts into spindle
speed (rpm)
Commands other than
G96
G96
command
Specified
Apply the
specified
surface
speed
Specify the
surface
speed
Without
specification
Employ the stored surface
speed mm/min (inch/min). 0 is
assumed if there is no stored
surface speed.
Fig. 6-3-3
180
Chapter Six Spindle Function S Code
6. The relative parameter setting of G96: When the bit 2 of parameter No.:37 sets the G0 at the
rapid traverse rate, calculate the reference coordinate of G96 spindle speed (0: End, 1:
Current point). When the bit 3 of parameter No.: 37 sets the G96 spindle speed clamping (0:
Before the spindle override, 1: After the spindle override); whether the setting of bit 0 of
parameter No.:61 is used the constant cycle speed control.
Restrictions:
1. The response problem in the servo system does not consider when the spindle speed changes,
but the constant surface cutting speed control is also enabled during thread cutting. And
therefore, cancel the constant surface cutting speed by G97 before the machining of thread.
2. In a rpaid traverse block specified by G00, the constant surface speed control is not made by
calculating the surface speed to a transient change of the tool position, but is made by
block, on the condition that cutting is not executed at rapid traverse.
3. When the machining, such as the flexible tapping, rigid tapping or peck tapping, etc. are
performed, it is necessary to firstly cancel the constant surface cutting feed by G97;
otherwise, the disorder gear or broken screw tap, etc. will occur.
181
VOLUME I
PROGRAMMING
calculating the surface speed based upon the position at the end point of the rapd traverse
GSK218MC Series Machining CNC System
VOLUME I
PROGRAMMING
182
Programming & Operation Manual
Chapter Seven Feed Function F Code
CHAPTER SEVEN
FEED FUNCTION F CODES
Feed function controls the feedrate of a cutter, the feed function and its control method are
shown below:
7.1
Rapid Traverse
The rapid positioning is performed by code (G00). The rapid feedrate are set by data parameter
P88~P92. The following override adjustment can be performed by its corresponding buttons on the
VOLUME I
PROGRAMMING
operation panel:
218MC, 218MC-H, 218MC-V buttons
218MC-U1 button
Fig. 7-1-1 The buttons of rapid feedrate
Wherein, F0: It is set by data parameter P93.
The acceleration of rapid positioning (G0) can be determined by data parameter P105~P123,
which can be set reasonably based upon the machine tool and the motor’s response characters.
Note: In the G00 block, the F code is disabled even if the it is specified; the system positions at the
G0 speed.
7.2
Cutting Speed
In the linear interpolation (G01) and circular arc interpolation (G02,G03), the feedrate of cutter is
specified by the numerical values followed with the F code, its unit is mm/min. Tool moves along the
cutting feedrate compiled in program. The cutting feedrate can be carried out by using the feedrate
buttons on operation panel (the override adjustment range is 0%～200%).
183
GSK218MC Series Machining CNC System
Programming & Operation Manual
Automatically perform the acceleration/deceleration to prevent the mechanical vibration at the
beginning and the end of the tool movement; acceleration can be set by data parameter P125~P128.
The Max. cutting speed is set by data parameter P96; The Min. cutting feed is determined by
data parameter P97; if the cutting feed is higher the Max restriction value, it will be restricted at the
upper-limit value; if the cutting speed is lower the Min. restriction value, it will be restricted at the
lower-limit value.
The cutting feedrate in the Auto mode, when the power is turned on, is determined by data
parameter P87.
The cutting speed can be specified by the following two methods:
A) Feed/min. (G94): Specify cutter feed value per minute after F.
B) Feed/rev. (G95): Specify the cutter feed value of the spindle per revolution after F.
VOLUME I
PROGRAMMING
Code format: G94
F_
Function: Feed amount per minute. Unit: mm/min or inch/min
Explanations:
1. After specifying G94 (in the feed per minute mode), the feed amount of tool per minute is
directly specified by the numerical value followed with the F.
2. G94 is a modal code. Once a G94 is specified, it is enabled until G95 is specified. It is
regarded as the feed per minute by default, and the default cutting feedrate is set by data
parameter P87.
3. The feed/min. can be debugged by override adjustment button or wave-band switch buttons
on the operation panel, the override is from 0% to 200%.
Feed amount per minute
mm/min or inch/min
Tool
Tool
Workpiece
Working table
Fig. 7-2-1-1 Feed per minute
7.2.2
Feed per Revolution (G95)
Code format: G95
F_
Function: Tool feed amount per revolution. Unit: mm/r or inch/r.
Explanations:
1. The machine tool can be used this function unless installing the spindle encoder.
184
Chapter Seven Feed Function F Code
2. The feed amount of per revolution is directly specified by the numerical values followed
with F after specifying G95 (feed/rev.) is specified.
3. G95 is modal code. Once a G95 code is specified, it is always enabled untill G94 is
specified. The default feedrate per revolution is zero in the initialization.
4. The feed/min. can be debugged by override adjustment button or wave-band switch
buttons on the operation panel, the override is from 0% to 240%.
Spindle feed amount
per revolution
(mm/rev. or inch/rev.)
F
Notice: When the speed of the spindle is low, feedrate fluctuation may occur. The slower the spindle rotates, the
more frequently feedrate fluctuation occurs.
Note: In the G95 feed per revolution mode, the top speed per revolution treated by system is F500, if it exceeds F500,
the alarm may issue.
7.3
Tangential Speed Control
Usually, the cutting feed is the speed for controlling contour path tangential direction, so that it can
be reached to the speed value of a command.
Y
Y
Start
End
FY
FY
Linear interpolation
F
End
F
Start FX
FX
X
X
Circular arc interpolation
Fig. 7-3-1
F: The speed along the tangential direction F= FX2+FY2+FZ2
Fx: The speed along the X axis direction
Fy: The speed along the Y axis direction
Fz: The speed along the Z axis direction
185
VOLUME I
PROGRAMMING
Fig. 7-2-2-1 Feed per revolution
GSK218MC Series Machining CNC System
7.4
Programming & Operation Manual
Feedrate Override Button
The feedrate in the Manual and Auto modes can be adjusted by the override adjustment buttons
on the operation panel, which can be used the override between 0～200% (10% of each gear, total
21 gears). In the Auto mode, when the override button adjusts to zero, the system will then stop the
feed, and displays the cutting override 0, and then adjust the override button, the program can be
continued.
7.5
Automatic Acceleration/Deceleration
VOLUME I
PROGRAMMING
The system is automatically performed the acceleration/deceleration control by moving the motor
at the start and end, and therefore, it can be stably started and stopped. Also, it can be automatically
accelerated or decelerated when the movement speed changes. Hernce, the acceleration or
deceleration does not consider when programming.
Rapid
feed:
Forward
acceleration/deceleration
(0:
Linear;
1:
S
type),
backward
Linear;
1:
S
type),
backward
acceleration/deceleration (0: Linear; 1: Exponential type)
Cutting
feed:
Forward
acceleration/deceleration
(0:
acceleration/deceleration (0: Linear; 1: Exponential type)
Manual feed: Backward acceleration/deceleration (0: Linear; 1: Exponential type)
(The general-purpose time constant along each axis can be set by parameter)
186
Chapter Seven Feed Function F Code
Speed followed with the interpolation
Speed
Speed after the
acceleration/deceleration control
Time
Speed
VOLUME I
PROGRAMMING
Time
TR
TR
Rapid traverse
Speed
TC: The acceleration/deceleration
time constant of cutting feed and
manual feed
(Data parameter 125-128)
TC
Cutting feed/manual feed
TC
Time
Fig. 7-5-1
7.6
Acceleration/Deceleration Treatment at Corner of Block
For example, if the previous block is only moved along Y, and the next block is only moved
along X; the X line accelerates while the Y decelerates, in this case, the tool path is as
follows:
187
GSK218MC Series Machining CNC System
Programming & Operation Manual
Insert a exact stop command
Y
(2)
Programmed path
The actual tool path
(1)
X
Fig. 7-6-1
If the exact stop code is input, the tool operates according to the program command as the solid
VOLUME I
PROGRAMMING
line in the Fig.7-6-1. Otherwise, the bigger the cutting speed is, or the longer the
acceleration/deceleration time constant is, the bigger the arc at the corner is. In the circular arc
command, the arc radius of the actual tool path is smaller than the one provided by program. If you
want to shorten the error at the corner, the acceleration/deceleration time constant should be set
smaller as much as possible in the case of the available mechnical system.
188
Chapter Eight Tool Function
CHAPTER EIGHT TOOL FUNCTION
8.1 Tool Function
Specify the numerical values (up to 8 digits) followed with the address T for using selecting the
tool on the machine tool.
In principle, two or more T codes can not be specified at a same block. If a same codes at a
same block is set without alarm, it is subject to the following T codes. The digit numbers to be
specified of address T and the machine tool operation of corresponding by T code can be referred to
When the movement codes and the T codes are specified at a same block, which are performed
at the same time.
When T codes and tool-change code M06 are shared with a same block, firstly perform the T
code, and then the tool-change code. If the T codes and tool-change code M06 are not shared with a
same block, the tool-change code detects whether the spindle tool number is consistent with the T
code cutter, if does, the tool-change will not be performed.
The following programs are regarded as examples:
O00010；
N10 T2M6；
The cutter on spindle is No.T2
N20 M6T3；
The cutter on spindle is No.T3
N30 T4；
The cutter on spindle is No.T3
N40 M6；
The cutter on spindle is No.T4
N50 T5；
The cutter on spindle is No.T4
N60 M30
%
The cutter on the spindle is No. T4 after the tool-change programs are performed.
189
VOLUME I
PROGRAMMING
the manual made by machine tool factory.
GSK218MC Series Machining CNC System
VOLUME I
PROGRAMMING
190
Programming & Operation Manual
Chapter One Operation Panel
VOLUME TWO
OPERATION
VOLUME II
OPERATION
191
GSK218MC Series Machining CNC System
VOLUME II
OPERATION
192
Programming & Operation Manual
Chapter One Operation Panel
CHAPTER ONE
1.1
OPERATION PANEL
Panel Classification
GSK218MC series contains of GSK218MC, GSK218MC-H, GSK218MC-V and GSK218MC-U1;
wherein, GSK218MC and GSK218MC-U1 CNC system are used the assembly structure,
GSK218MC-H and GSK218MC-V are separately used the horizontal structure and vertical structure.
Panel divides into LCD area, Editing keyboard area, sofkey function area and machine tool control
area; refer to the following figures:
LCD display area
Edit keyboard area
VOLUME II
OPERATION
Soft key function area
Fig. 1-1-1
Machine control area
GSK218MC panel
193
GSK218MC CNC System Programming & Operation Manual
VOLUME II
OPERATION
Fig. 1-1-2
194
GSK218MC-H panel
Chapter One Operation Panel
VOLUME II
OPERATION
Fig. 1-1-3
GSK218MC-V panel
195
GSK218MC Series Machining Center CNC System Programming & Operation Manual
LCD display area
Editing keyboard area
VOLUME II
OPERATION
Softkey function area
Machine tool control area
Fig. 1-1-4
1.2
1.2.1
GSK218MC-U1 panel
Panel Function Explanation
LCD Display Area
GSK 218MC and GSK 218MC-V systems are used the colorful 10.4 inch LCD with 800×600
resolution.
GSK 218MC-H and GSK 218MC-U1 systems are used the colorful 8.4 inch LCD with 800×600
resolution.
196
Chapter One Operation Panel
1.2.2
Editing Keyboard Area
VOLUME II
OPERATION
Fig. 1-2-2-1
GSK218MC及GSK218MC-H Editing keyboard area
3
1
2
4
9
5
8
7
6
Fig. 1-2-2-2
10
GSK218MC-V Editing keyboard area
197
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 1-2-2-3
GSK218MC-U1 Editing keyboard area
In the editing keyboard area, the function of buttons are divided into 10 areas again; the concrete
usages are shown below:
VOLUME II
OPERATION
Series
Description
Function Explanation
1
Resetting button
System resets, feed or output stops.
2
Address button
Enter the MDI addresses
3
Number button
Enter the MDI numbers
4
Input button
No.
5
6
7
Input the numbers, addresses or data to the buffering area to
confirm the operation result
Screen operation
Control any of the buttons, enter to the corresponding interface
button
display. (Refer to the CHAPTER THREE for details)
Page button
Cursor movement
button
8
Editing button
9
Searching button
It is used for the page shifing and the page up/down of program
in the same display mode.
It is used for moving the cursor up/down or left/right.
It can be moved the cursor to the start or end of the program line
and the program.
It is used for searching the data, address to check or modify.
It is used for operations, suchas the insertion, modification or
10
Editing button
deletion of program or word field, etc. as well the usage of
complex buttons when the program is compiled.
198
Chapter One Operation Panel
1.2.3
Introduction of Screen Operation Buttons
There are 8 operation page display buttons and one help page display key are displayed on
operation panel for this system, refer to the following figure:
Graphic page
System page
Descript
Function
ion
Explanation
Alarm page
Help page
Position page Program page
PLC page
Diagnosis page
Setting page
Remark
Display the graph parameter and its graph display page by the
Graph
Enter the
page
graph page
corresponding softkey conversion.
The graph parameter sets the graph center display, dimension
and proportion.
Enter the
page
alarm page
Help
Enter the help
Check different help information by converting the corresponding
page
page
softkey.
Program
Enter
-control
program-contr
page
Diagnosi
s page
the
ol page
Enter the
diagnosis
page
System
Enter the
interface
system page
Position
Enter the
page
position page
Program
Enter the
page
program page
Setting
Enter the
page
setting page
Check different alarm information pages by converting the
VOLUME II
OPERATION
Alarm
corresponding softkey.
Check the configutration of the relevant version information and
system I/O port of the PLC ladder diagram by corresponding
softkey conversion; simultaneously, the PLC ladder diagram can
be altered in MDI mode.
Check the I/O port signal state at each side of system by
corresponding softkey conversion.
Display cutter offset, parameter, macro variable and screw
compensation display pages by the corresponding softkey
conversion.
Display the relative, absolute, complex and program-monitoring
display pages by the corresponding softkey conversion.
Display the program, MDI, CUR/MOD, CUR/NXT, list display
page; the multi-page program names can be checked by the
page buttons on the list interface.
There are 4 interfaces, such as the display setting, workpiece
coordinate, data and password setting, which can be converted
by corresponding softkey.
199
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Note: The above-mentioned each softkey conversion interface can also be carried out by using the consecutive
corresponding function buttons based upon the setting of bit 0~7 of parameter No.:25 and bit 6~7 of parameter
No.: 26. Refer to the CHAPTER THREE of this manual for the details.
1.2.4
GSK218MC Machine Tool Control Area
Fit. 1-2-4-1
VOLUME II
OPERATION
200
GSK218MC Machine control area
Chapter One Operation Panel
Button
Description
Function
Remark & Operation
Indicator is ON when
the dry run is enabled.
Auto, MDI, DNC
Indicator is ON when
Miscellaneous MST function is ON, M,
function switch S a n d T f u n c t i o n
outputs are disabled.
Auto, MDI, DNC
Dry run switch
Indicator is on when
Auto, MDI, Mechanical
Machine lock machine locking is ON; zero, MPG, Single-step,
t
h
e
a
x
i
s
o
p
e
r
a
t
i
o
n
switch
Manual and DNC
output is disabled.
M a c h i n e Machine working
w o r k i n g indicator ON/OFF
indicator switch
Lubrication
switch button
Machine lubrication
ON/OFF
Any mode
Any mode
Coolant ON/OFF
Any mode
Chip-removal
switch button
Chip-removal
ON/OFF
Any mode
S p i n d l e
control button
Spindle positive
Spindle stop
Spindle reverse
Spindle speed adjustment
Spindle override ( T h e s p i n d l e s p e e d
analog value control
button
VOLUME II
OPERATION
Coolant switch
button
MPG mode, single-step
mode and manual mode
Any mode
method is enabled)
Spi ndl e JOG S p i n d l e J O G s t a t e
ON/OFF
switch
Spi ndl e ex act
stop button
Manual mode, singlestep mode and MPG
mode
Spindle exact stop
Manual mode, single-step
ON/OFF
mode and MPG mode
Tool-magazine T o o l m a g a z i n e Manual mode
operation button operation ON/OFF
M a n u a l M a n u a l
r e l e a s i n g / r e l e a s i n g / c l a m p i n g Manual mode
clamping switch switch
201
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
Note: When the symbol numbers at the beginning of a block is more than 1, that is, the enabling skip function
does not open, the system then skips this block.
202
Chapter One Operation Panel
1.2.5
GSK218MC-H and GSK218MC-V Machine Tool Control Area
GSK218MC-H Machine tool control area
Fig. 1-2-5-2
GSK218MC-V Machine tool control area
VOLUME II
OPERATION
Fig. 1-2-5-1
The usages and function definitions of the basis buttons on the GSK218MC-H and GSK218MC-V
machine tool control area are absolutely coincided with the GSK 218MC. Here, we just describe the new
additional buttons:
203
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Button
Description
ESP button
To make the system
entering the ESP
state
Remark & Operation
Any mode
N axis selection A x i s s h i f t i n g f o r
multi-axis
button
Manual mode, single
mode and MPG mode
Spindle speed
adjustment (The
Spindle override spindle speed analog
switch
value control method
is enabled)
Any mode
Feed override
switch
VOLUME II
OPERATION
1.2.6
Function
The adjustment of Auto mode, MDI mode,
Manual mode and DNC
feedrate
mode
GSK218MC-U1 Machine Tool Control Area
Fig. 1-2-6-1
GSK218MC-U1 Machine tool control area
The usages and function definitions of the basis buttons on the GSK218MC-U1 machine tool control
area are basically coincided with the GSK 218MC. Here, we just describe the differences between
GSK218MC-U1 and GSK218MC:
204
Chapter One Operation Panel
Button
Function
Description
Remark & Operation
Tool-magazine T o o l m a g a z i n e There is no tool-magazine
relevant button from
operation button operation ON/OFF
218MC-U1.
Manual
M a n u a l There is no tool
releasing/clampin releasing/clamping releasing/clamping button
g switch
switch
from 218MC-U1.
M a n u a l t o o l - C o m p l e t e t h e There is no manual toolchange button from
change
manual tool-change 218MC-U1
The shifting of
C h a n n e l machining channel T h e r e i s n o f u n c t i o n
selection button (This function does button for 218MC-U1
not perform yet)
Rapid override,
Manual single and
MPG override
selection buttons
Auto, MDI, Mechanical
zero, MPG, Single-step,
Manual and DNC . The
button function of 218MCU1 is coincided with the
218MC, other than the
button icons.
VOLUME II
OPERATION
Rapid override,
ma n u a l s i n g l estep and MPG
override selection
buttons
Any mode
M o v e m e n t R a p i d t r a v e r s e The button function of
218MC-U1 is coincided
override button
ON/OFF
with the 218MC, other
than the button icons.
X, Y, Z and the 4th axis
m
o
v
e
s
positively/reversely
in
Manual feed
manual, single-step
button
oper at ion methods ;
positive axis regards
as MPG selection axis.
Note 1: The feed hold button
and cycle start button
shared the same effect with the
and
Mechanical zero, Singlestep, Manual and MPG.
The button function of
218MC-U1 is coincided
with the 218MC, other
than the button icons.
of GSK218MC and GSK218MC-U1 are
of GSK218MC-H and GSK218MC-V. The
following introduction of the buttons of 218MC are regarded as an example.
Note 2: In Manual mode, the manual speed override is adjusted by the feed override switch in the case of the rapid
traverse buttons are not controlled.
Note 3: The buttons within the < >, in the following explanations, are regarded as panel buttons; within the【 】are
205
GSK218MC Series Machining Center CNC System Programming & Operation Manual
treated as softkeys below the screen;【 】is the corresponding interface for the current softkeys;
that there is sub-menu within this menu.
VOLUME II
OPERATION
206
means
Chapter Two System ON/OFF & Safety Operation
CHAPTER TWO
2.1
SYSTEM ON/OFF & SAFETY OPERATION
System ON
The following items should be confirmed before the power of the GSK218MC CNC system
turned on.
1. The machine tool state should be normal.
2. The power voltage should be conformed with the requirements.
3. The wiring should be correct and firm.
The current position (relative coordinate) page displays after the system self-checking is normal,
and the initialization is completed.
VOLUME II
OPERATION
Fig. 2-1-1
2.2
Power OFF
It is necessary to confirm the following items before the power is turned off.
1. The X, Y and Z axes of the CNC are on the stop state;
2. The miscellaneous functions (such as spindle, water-pump, etc.) are closed;
3. Firstly cut off the power of CNC, then the machine tool.
The following inspections should be performed when the power is turned off:
1. The LED cycle start on the operation panel should be located at the stop state;
2. The overall movable components of the CNC machine should be on stop state;
3. Turn off the machine by POWER OFF button.
Cut off the power in an emergency
207
GSK218MC Series Machining Center CNC System Programming & Operation Manual
The power of machine tool should be cut off immediately in case of emergency during the
operation of the machine for avoiding an accident. However, it is very important to note that the
system coordinate may offset to the actual position after the power is turned off; and therefore, the
operations such as the zero, tool-setting, etc. should be performed again.
Note: Refer the operation for cutting off the machine power based upon the Machine Tool User Manual manufactured
by the factory.
2.3
Safety Operation
2.3.1
Resetting Operation
The system is on the resetting state after pressing
.
1. The movement of overall axes are stopped.
2. M function stops.
3. Modify the bits 1～7 of parameter No.: 35 and bits 0～7 of parameter No.:36; set whether
VOLUME II
OPERATION
the G codes of each group is reserved after resetting.
4. Modify the bit 7 of parameter No.:34; set whether cleans the F, H and D codes after
reseeting.
5. Modify the bit of parameter No.: 28; set whether delects the compiled program after
resetting in the MDI mode.
6. Modify the bit 3 of parameter No.: 10; set whether cancels the relative coordinate system
after resetting.
7. Modify the bit 7 of parameter No.: 10; set whether the resetting cursor turns to the
beginning of the program in the non-compiled method.
8. Modify the bit 7 of parameter No.: 52; set whether cleans the macro program local variable
#1～#50 after resetting.
9. Modify the bit 6 of parameter No.: 52; set whether cleans the macro program common
variable #100～#199 after resetting.
10. It can be used in the system output abnormality and coordinate axis abnormality.
2.3.2
ESP
The system enters the ESP state after pressing the ESP button during the machine tool is being
operated. In this case, the machine tool is immediately stopped. The ESP can be removed after
releasing this button (Although it differs depending on the manufactures, usually, rotate this button left,
it can be automatically skipped).
208
Chapter Two System ON/OFF & Safety Operation
Note 1: It is necessary to confirm that the fault reason is eliminated or not before releasing the ESP button.
Note 2: Perform the reference point return operation again after the ESP button is released to ensure the correct of
the coordinate position.
Generally, the ESP signal is NC contactor signal, when the contractor is cut off, the system then
enters the ESP state, and the machine is emergently stopped accordingly. The ESP circuit
connenction is shown below:
+24V
ESP button
ESP
Fig. 2-3-2-1
2.3.3
Feed Hold
during the operation of the machine tool. It is essential to note
that the dwells performs after the current codes are carried out in the rigid tapping or cycle code
operation.
2.4 Cycle Start & Feed Hold
In the controllable panel,
and
are used for the program’s start and dwell in
Auto, MDI and DNC modes. Set whether uses the external start and dwell by modifying the K5.1 in
the PLC address.
Note 1: The shifting is performed among the Auto, MDI and DNC modes. The cycle start is enabled before the current
block is performed, and the feed hold is disabled by the <FEED HOLD> button.
Note 2: Shift to editing mode in the Auto, MDI and DNC modes. The cycle start is disabled before the current block is
performed, and the feed hold is disabled by the <FEED HOLD> button.
Note 3: Shift to machine tool zero return, single step, manual and MPG modes in the Auto, MDI and DNC modes. The
feed hold is disabled by the <FEED HOLD> button.
Note 4: In the cycle start mode, when shifting among the Auto, MDI and DNC modes or when the shifting is editing
mode. Press the <FEED HOLD> button before performing the current block, and the feed hold function is on
the disabled state.
209
VOLUME II
OPERATION
The operation dwell by
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2.5 Overtravel Defense
To avoid the machine damage due to the X axis, Y axis and Z axis are exceeded the overtravel,
and the machine should be taken the overtravel defense measure.
2.5.1
Hardware Overtravel Defense
Separately install the stroke limit switch at the Max. stroke with positive or negative along the X
axis, Y axis or Z axis, when the overtrvel occurs, the operation axis decelerates and stops eventually
after touching the limit switch, the system then prompts the overtravel alarm information.
Decelerates till stops
Tool
Tool
Limited switch
Y
X
VOLUME II
OPERATION
Fig. 2-5-1-1
Detailed explanations:
The overtravel in the Auto mode
In the Auto mode, when the tool touches the limit switch moves along one axis, the overall axes
operations may decelerate and then stop; simultaneously, the overtravel alarm occurs, and the
program stops at the overtravel block.
The overtravel in the Manual mode
In the manual operation, as long as any axis of the machine tool touches the limit switch, the
operations of the overall axes will be immediately decelerated then stopped.
2.5.2
Software Overtravel Defense
The software stroke range is set by data parameter P66~P73, and the machine tool coordinate
value is regarded as the reference value. If the movement axis exceeds the soft limit parameter
setting, the overtravel alarm may occur. The bit 6 of parameter No.: 11 sets whether the stroke
inspection (0: No, 1: Yes) is performed after the power is turned on till to the manual reference
position return. When the bit 7 of parameter No.: 11 sets the soft limit overtravel, the overtravel (0:
Before, 1: After) alarms. The overtravel moves the axis reversely in the <Manual> mode, the alarm is
then released after moving out of the overtravel range.
210
Chapter Two System ON/OFF & Safety Operation
2.5.3
Releasing of Overtravel Alarm
The method for releasing the hard limit overtravel: In the manual or MPG mode, firstly press the
on the panel, then move out the axis (For example, if it is positive overtravel, it moves out
toward to negative, vice versa) reversely.
2.6 Stroke Inspection
Two cutter forbidden areas can be specified by stored stroke detection 1 and 2.
(X,Y,Z)
(I,J,K)
(1) The interior is forbidden area
(X,Y,Z)
VOLUME II
OPERATION
(I,J,K)
(1) The exterior is forbidden area
: the forbidden area of cutter
Fig. 2-6-1 Stroke inspection
When the tool exceeds the stored stroke limit, the alarm displays and the machine tool
decelerates then stops.
When the tool enters the forbidden area and alarm occurs, the tool can be moved along the
reverse direction when it enters.
Detailded explanations:
1. Stored stroke detection 1: This boundary can be set by data parameter P66~P73, the exterior of
this area is forbidden one. The manufacturer, usually, sets this area as the Max. stroke of the
machine tool.
2. Stored stroke detection 2: Data parameter P76~P83 or the program code can be set this
boundary, the area within this boundary or out of the boundary can be set as the forbidden area,
which is set by bit 0 of parameter No.: 11 (0: The forbidden area is inside; 1: The forbidden area is
outside).
1) When the parameter setting forbidden area is used: the points A and B should be set in the
following figure.
211
GSK218MC Series Machining Center CNC System Programming & Operation Manual
A (X,Y,Z)
B (I,J,K)
X>I,Y>J,Z>K
X-I> (The least command incremental unit)
Y-J> (The least command incremental unit)
Z-K> (The least command incremental unit)
Fig. 2-6-2
Establish or change the forbidden area by parameter
When the forbidden area is set by setting the data parameter P76~P83, the data should be
offered the distance (output increment) to the machine tool coordinate with the least command
incremental unit.
2) When the program is used: G12 prohibts the cutter to enter the forbidden area; G13 allows the
VOLUME II
OPERATION
cutter to enter the forbidden area.
Each G12 in program should be specified by a separated block, the following commands are used
for establishing or changing the forbidden area.
G12 X
Y
Z
I J K _;
A (X,Y,Z)
B (I,J,K)
X>I,Y>J,Z>K
X-I> (The least com m and increm ental unit)
Y-J> (The least com m and increm ental unit)
Z-K> (The least com m and increm ental unit)
Fig. 2-6-3 Establish or change the forbidden area by program
The distance (input increment) in the machine tool coordinate system is specified by the least
input incremental unit based upon the setting of the G12.
The programmed data is the digit value of the least code unit converted from the least
incremental unit, and this value is then set in the parameter.
Example: The forbidden area is inside (bit 0 of parameter No. 11=0):
212
Chapter Two System ON/OFF & Safety Operation
N1 G12 X50 Y40 Z30 I20 J10 K15;
Set the tool forbidden area point A (5,
40, 30), B (20, 10, 15).
N2 G01 X30 Y30 Z20;
Linear interpolation to (30, 30, 20)
N3 G13;
Cancel the stored stroke detection
fuction
N4 G01 X50;
Example 2: The forbidden area is outside (bit 0 of parameter No.: 11=1):
N1 G12 X50 Y40 Z30 I20 J10 K15;
Set the tool forbidden area point A (50,
40, 30), B (20, 10, 15).
N2 G01 X10 Y-10 Z-10;
Linear interpolation to (10, -10, -10)
N3 G13;
Cancel the stored stroke detection
fuction
N4 G01 X50;
3) The inspection point of forbidden area: It is important to confirm the inspection point position (the
top of the tool-nose or tool-setting) before programming the forbidden area. Refer to the Fig. 2-6-4,
for example, the inspection point A (tool-nose), the distance “a” should be set as the data of the
stored function inspection; the point B (tool-setting), the distance “b” should be set as the data of
varies from different tools, the forbidden area should be set based upon the longest tool to
guarantee the safety operation.
Tool position after
reference point return
Tool
b
B
A
a
Area
boundary
: the forbidden area of tool
Fig. 2-6-4 Set the forbidden area
4) The overlap of tool forbidden area: the forbidden area can be set by the overlapping method.
Refer to the following figure:
213
VOLUME II
OPERATION
the stored function inspection. When the inspection point is A (tool-nose), and the tool length
GSK218MC Series Machining Center CNC System Programming & Operation Manual
: the forbidden area of tool
Fig. 2-6-5 Set the overlapped forbidden area
The unnecessary limit should be set out of the stroke of the machine tool.
5) When bit 6 of parameter No.: 11=0, the enabled time of forbidden area: after the power is
turned on, the manual reference position return is performed or the automatic reference point
return is performed by G28, the forbidden area bundary is then enabled inmmediatly.
When the bit 6 of parameter No.: 11 =1, after the power is turned on, if the reference position
is within the forbidden area, it may alarm immediately, (It is only enabled in the G12 mode in
the stored stroke limit 2).
6) Alarm releasing: If it enters the forbidden area and the alarm occurs, the tool is only moved
VOLUME II
OPERATION
toward the reverse direction. In order to eliminate the alarm, the tool moves along its negative
direction, till retreating from the forbidden area, and the system is then reset. The tool can be
moves forward or backward after the alarm removes. Refer to the Section 2.5.2 in this operation
maual for detail.
7) The alam may immediately occur in forbidden area when G13 converts into G12.
8) The bit 1 of parameter No.:10 sets the movement whether performs the stroke inspection.
When bit 1 of parameter No.: 10 equals to 0, the stroke inspection does not perform before
moving; when bit 1 of parameter No.: 10 equals to 1, the stoke inspection is performed before
moving.
214
Chapter Three
CHAPTER THREE
Interface Display & Data Modification & Setting
INTERFACE DISPLAY & DATA MODIFICATION
AND SETTING
3.1 Position Display
3.1.1 Four Methods of Position Page Display
Enter the position page display by
. There are four position display pages: 【RELATIVE
COORDINATE】, 【ABSOLUTE COORDINATE】,【COMPOSITIVE】,【PROGRAM MONITORING】,
which can be viewed by the corresponding softkeys; refer to the following:
1) Relative coordinate: Display the position of the current tool at the relative coordinate system by
the 【RELATIVE COORDINATE】softkey. (Refer to the Fig. 3-1-1-1).
VOLUME II
OPERATION
Fig. 3-1-1-1
2) Absolute coordinate: Display the position of the current tool at the absolute coordinate system
by the 【ABSOLUTE COORDINATE】softkey. (Refer to the Fig. 3-1-1-2).
215
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-1-1-2
3) Compositive: Enter the interface by 【COMPOSITIVE】softkey, they will be displayed at the
same:
(A) The position at the relative coordinate system;
(B) The position at the absolute coordinate system;
VOLUME II
OPERATION
(C) The position at the machine coordinate system;
(D) The offset in the MPG interruption (Shift value);
(E) Velocity component;
(F) Remainder movement value (It displays in the Auto, MDI and DNC mode)
The display page is as follows: (refer to the Fig. 3-1-1-3):
Fig. 3-1-1-3
4) Program-monitoring method
216
Chapter Three
Interface Display & Data Modification & Setting
Enter the 【PROGRAM-MONITORING】interface by its software, in this interface, the current
position absolute coordinate, relative coordinate can be simultaneously displayed with the modal
information and operation block at the current operation. (Refer to the Fig. 3-1-1-4)
Note 1: Whether the modal in the program-monitoring display interface can be displayed by bit 6 of parameter No.: 23.
When BIT6=0, the modal code does not display on the interface instead of displaying the machine tool
coordinate value at the original position.
Note 2: In the <Zero>, <Single-step>, <Manual> and <MPG> modes, the intermediate coordinate system is regarded
as the relative one; in the <Auto>, <MDI> and <DNC> modes, the intermediate coordinate system is treated as
the remainder movement amount.
3.1.2 Display Machining Time, Component Numbers, Programming Speed,
Override and Acutal Speed, Etc. Information
【RELATIVE】method interface displayed from <Position>, the information,
In the 【ABSOLUTE】
such as the programming speed, actual rate, feedrate, rapid override, G function code, tool offset,
machining numbers, cutting time, spindle speed override, spindle speed and machining tool, etc. can
be displayed; refer to the Fig. 3-1-2-1:
217
VOLUME II
OPERATION
Fig. 3-1-1-4
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-1-2-1
The concrete meanings are shown below:
Rate: The actual machining rate after the override is performed during the machining.
Programming rate: The rate specified by F code code in a program.
Feedrate: The selected override by feedrate switch.
VOLUME II
OPERATION
Rapid override: The override controlled by system default panel, or the selected override by
rapid traverse wave band switch.
G function code: The value of the G code is being performed at present.
Tool offset: The tool length compensation of the current H0000 machining program; The radius
compensation of the current H0000 machining program.
Machining numbers: When machining number of the program adds 1 and perform to M30 or M02
in the Auto or DNC mode, the other modes will not add.
Cutting time: When the Auto operation starts, the timing begins, and its unit is hour, minute and
second in turn.
S00000: Command speed. Cursor positions at the “S00000” (Spindle speed) after pressing the
direction button
in the relative, absolute coordinate page; in this case, the S
value can be modified (the alteration range is the setting value from 0 to data
parameter P258).
T0000: The tool number specified by T code in program.
Note: The machining numbers are memorized after thw power is turned off.
The zering method of machining number, cutting time:
1) Shift to the position interface, then select the MDI mode.
218
Chapter Three
Interface Display & Data Modification & Setting
2) Cursor positions to the machining number column after controlling the direction button
, the data can be input and then press the
numbers will be cleared if directly press the
to confirm; the machining
.
3) Shift to cutting time by up/down buttons.
4) Press the
: Cutting time clears.
Note 1: There is no alternative other than to install the encoder on spindle when the actual speed of the spindle is
displayed.
Note 2: Actual rate = the F value of programming rate × override. In the G00, the operation speed of each axis is
set by data parameter P88～P92, which can be adjusted by rapid override; and the dry run speed can be
determined by data parameter P86.
Note 3: The programming rate display of feed per revolution: It displays that the block contains each feed per
revolution is being performed.
Note 4: The machined total components can be set by data parameter P356, the desired machining total
components can be set by data parameter P357.
VOLUME II
OPERATION
3.1.3 Relative Coordinate Clear and Middle
The relative coordinate position clears, the operation steps are shown below:
1) Enter any interface with the relative coordinate display (Refer to the Fig. 3-1-3-1)
Fig. 3-1-3-1
219
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2) Clearing operation: The X flashes by the “X” button, then press the
, in this case, the
relative coordinate value towards to the X is already cleared (Refer to the Fig. 3-1-3-2);
VOLUME II
OPERATION
Fig. 3-1-3-2
3) Middle Operation: The X flashes by the “X” button, then press the
, in this case, the
relative coordinate value towards to the X is already divided at the middle (The relative
coordinate value of this axis is divided by 2);
4) Coordinate setting: The X flashes by the “X” button, then input the desired data confirming
by
, the data is inputted to the coordinate system accordingly.
5) The clearing method of the Y and Z axes are identical with the above-mentioned.
3.1.4 Bus Monitoring Position Page Display
When the system uses the Ethernet bus communication method, enter the position page display
by
, then the 【MONITORING】interface by its softkey; in this interface, simultaneously, the
current machine coordinate, multi-coil position, encoder value, grating position, motor speed and
motor loanding (% means the percentage of the rated loading) can be display. It is convenient to
debug the machine and monitor the servo current operation state with real-time by this interface.
(Refer to the Fig. 3-1-4)
220
Chapter Three
Interface Display & Data Modification & Setting
VOLUME II
OPERATION
Fig. 3-1-4-1
3.2 Program Display
Enter the program page display by the
on the panel, there are five interfaces:【
PROGRAM】,【MDI】,【CUR/MOD】,【CUR/NXT】and 【LIST】, which can be viewed and altered
by the corresponding softkeys, refer to the Fig. 3-2-1 is as follows:
1) Program display
Enter the program display page by【
PROGRAM】softkey, in this page, the program at the
page of the block is being performed that displays inside the memory (Refer to the Fig. 3-2-1).
221
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-2-1
Press the【
PROGRAM】again, the editing and modification pages of the program are shown
in this interface (Refer to the Fig. 3-2-2):
VOLUME II
OPERATION
Fig. 3-2-2
Press【X】 enter to next page
Press 【X】enter to next page
Press【(】 return to previous page
Note: Wherein, 【CORRECTION】function can only be used in the Auto mode.
【B.EDITING】and【B.END】can only operate this function (Background editing function) in Auto
222
Chapter Three
Interface Display & Data Modification & Setting
and DNC modes. The editing program of each function for 【 B.EDITING 】 is indentical in the
<EDITING> mode; refer to the Program Editing Operation of Chapter Ten of OPERATION. After the
editing is performed, save this editing interface by【B.END】 and retreating from it by【RETURN】.
2) MDI input display
Enter the MDI display interface by【MDI】softkey, in the MDI mode, multi-program can be
compiled and performed. The program format is as same as the editing program. MDI operation is
suitable for the simple testing program operation (Refer to Fig. 3-2-3).
VOLUME II
OPERATION
Fig. 3-2-3
4) Program (CUR/MOD) display
Enter the CUR/MOD display page by the【CUR/MOD】softkey, the code value is displayed for the
being performed block and the current modal value; the MDI data input and operation can be
performed in the MDI mode (Refer to the Fig. 3-2-4).
Fig. 3-2-4
223
GSK218MC Series Machining Center CNC System Programming & Operation Manual
4) Program (CUR/NXT) display
Enter the CUR/NXT display page by the【CUR/NXT】softkey, the code value is displayed for the
being performed block and the next block to be performed program (Refer to the Fig. 3-2-5).
Fig. 3-2-5
5) Program list display
VOLUME II
OPERATION
I. Enter the program (System list) display interface by【LIST】softkey, the display content is
shown below (Refer to the Fig. 3-2-6):
(a) Program numbers: the stored program number (include the subprogram) / the Max.
program numbers to be registered.
(b) Memory capacity: The occupied memory capacity/program storage total capacity for
the stored programs.
(c) Program list: Display the program number of the registered program in turn.
(d) Preview the program at the current cursor located.
Fig. 3-2-6
II. Enter the program (USB list) display interface by【LIST】softkey, the display content is as
224
Chapter Three
Interface Display & Data Modification & Setting
follows (Refer to Fig. 3-2-7).
Fig. 3-2-7
Explanation: The overall program numbers within the memory is displayed by the page buttons, the
VOLUME II
OPERATION
program names can not be viewed if they are more than 6-digit or improper the regular.
3.3 System Display
Enter the system page by
PARAMETER 】 , 【
, there are five sub-interface for this page: 【 OFFSET】,【
MACRO VARIABLE 】 , 【 PITCH COMPENSATION 】
and 【
BUS
CONFIGURATION】, which can be shifted and displayed by its corresponding software. Refer to the
following figure (Fig. 3-6-1):
3.3.1 Display, Modification and Setting of Offset
3.3.1.1 Display of Offset
Enter the offset display page by【 OFFSET】softkey, the offset interface is then shown below
(Refer to the Fig. 3-3-1-1-1):
225
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-3-1-1-1
Press the【 OFFSET】softkey in the above figure, then enter the operation interface. (Refer to
the Fig. 3-3-1-1-2)
VOLUME II
OPERATION
Fig. 3-3-1-1-2
The compensation value can be directly input or performed the addition/subtraction operation
with the value at the current position. Shape (H) means the tool length compensation; Wear (H)
means tool length abrasion and wear; Shape (D) meand cutter compensation; Wear (D) means cutter
radius abrasion and wear.
226
Chapter Three
Interface Display & Data Modification & Setting
3.3.1.2 Modification and Setting of Offset Value
The methods for setting the tool offset in the offset interface:
1) Enter the offset display interface by【 OFFSET】.
2) Move the cursor to the position where to be inputted the compensation number.
Method 1: Display the page to be modified the compensation value by page up/down button;
Move the compensation number position to be modified by cursor.
Method 2: After the compensation number is input, positioning performs by
3) Input the compensation value in any mode, and then confirm it by
.
or 【INPUT】softkey.
4) Input the compensation value in amy mode, and then press【+INPUT】or【-INPUT】softkey; the
system will then automatically calculate the compensation value and display it.
Note 1: When the tool offset is changed, the new offset value can be enabled, only when the specified H or D code of
compensation number shoul be performed.
Note 2: User can freely alter the tool compensation value during the program operation. When, however, the
modification should be completed before performing this tool compensation number, if it can be immediately
Note 3: For example, the length compensation value shold be added the relative coordinate value of the Z axis; it is
only need to be write the compensation value followed with the Z axis, the system will then automatically overlapped.
For instance, input the Z 10, the compensation value is regarded that the current relative coordinate value of Z
axis adds 10.
3.3.2 Display, Modification and Setting of Parameter
3.3.2.1 Parameter Display
Enter the parameter page display by【
PARAMETER】, there are two sub-interface within the
parameter page: 【BIT PARAMETER】,【DATA PARAMETER】, which can be viewed or altered by
its corresponding softky, is as follows:
1) Bit parameter page
Enter the bit parameter interface by【BIT PARAMETER】. (Refer to the Fig.
3-3-2-1-1)
227
VOLUME II
OPERATION
enabled during program operation.
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-3-2-1-1
Refer to the Appendix One Parameter Explanation for the concrete definitions of each
parameter.
2) Data parameter page
Enter the data parameter page by【DATA PARAMETER】softkey. (Refer
VOLUME II
OPERATION
to the Fig. 3-3-2-1-2):
Fig 3-3-2-1-2
Refer to the Appendix One Parameter Explanation for the concrete definitions of each
parameter.
228
Chapter Three
Interface Display & Data Modification & Setting
3.3.2.2 Modification and Setting of Parameter Value
1) Select the <MDI> operation mode.
2) Enter the <SETTING> page by
3) Press
, then the【
, the parameter switch set to “1”.
PARAMETER】softkey, lastly enter the parameter display page.
4) Move the cursor to the position where the parameter number to be modified:
Method 1: Display the page to be set the parameter by page up/down button; move the
cursor bu direction buttons, and then position the parameter place to be modified.
Method 2: Press
to position after inputting the parameter number.
5) Input the new parameter value (It is necessary to input the password authority of the
corresponding level when different levels parameter are modified) by numerical button.
6) Press the
to confirm, the parameter value is input and then displays.
VOLUME II
OPERATION
7) Close the parameter switch after the overall parameters setting are completed.
3.3.3 Display, Modification and Setting of Macro Variable
3.3.3.1 Display of Macro Variable
Enter the macro variable page display by 【
MACRO VARIABLE 】 softkey, there are two
sub-interface within the macro variable page: 【USER VARIABLE】,【SYSTEM VARIABLE】, which
can be viewed or modified by its corresponding softkeys, refer to the following concrete descriptions:
1) User variable page
Enter the user variable interface by【USER VARIABLE】softkey. (Refer to
the Fig. 3-3-3-1-1):
229
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-3-3-1-1
2) System variable page
Enter the system variable page by 【SYSTEM VARIABLE】 (Refer to
VOLUME II
OPERATION
the Fig. 3-3-3-1-2):
Fig. 3-3-3-1-2
Refer to the Section 4.7.2
the macro variable.
230
Macro Variable in PROGRAMMING for the explanation and usage of
Chapter Three
Interface Display & Data Modification & Setting
3.3.3.2 Modification and Setting of Macro Variable
1) Select the <MDI>operation mode.
2) Press the
, then【
MACRO VARIABLE】softkey to enter the macro variable display
page.
3) Move the cursor to the position where the variable number to be modified:
Method 1: Display the page to be set the variable by page up/down button; move the cursor
bu direction buttons, and then position the variable place to be modified.
Method 2: Press the
to position after inputting the variable number.
4) Input a new numerical value by number buttons.
5) Confirm that the numerical value is input and displayed by
.
3.3.4 Display, Modification and Setting of Ptich Compensation
Enter the pitch compensation interface by 【 PITCH COMPENSATION 】 softkey, the pitch
compensation interface is as follows (Refer to the Fig. 3-3-4-1-1):
Fig. 3-3-4-1-1
231
VOLUME II
OPERATION
3.3.4.1 Pitch Compensation Display
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3.3.4.2 Modification and Setting of Pitch Compensation
1) The pitch error compensation number of each axis is set by data parameters P216～P220; the
pitch error compensation interval is set by data parameters P226～P230.
2) In the <MDI>, input the compensation amount of each point in turn.
Note: Refer to the INSTALLATION & CONNECTION of the Chapter Four in GSK218MC CNC System PLC &
Installation Connection Manual for the setting of the pitch compensation.
3.3.5 Display, Modification and Settong of Bus Servo Parameter
Enter the system page by
, display the【
BUS CONFIGURATION】sub-interface by its
corresponding softkey shifting. Refer to the following figure (Fig. 3-3-5-1):
VOLUME II
OPERATION
Fig. 3-3-5-1
【 BUS CONFIGURATION】Interface operation explanations
After entering the bus configuration interface by the【 BUS CONFIGURATION】softkey,as the
Fig. 3-3-5-1, the parameters displayed in this page can be viewed; as well, the relevant parameters
can be altered. The concrete operation methods and steps are shown below:
1. Ente <MDI> operation mode;
2. Move the cursor by the up/down/left/right direction buttons to the item to be modified.
3. Modification is performed based upon the following explanations;
1) Whether it is bus
0: Drive transmission method is pulse.
232
Chapter Three
Interface Display & Data Modification & Setting
1: Drive transmission method is bus.
Note: It can also be set as bus method by the bit 0 of parameter No.: 0.
2) Encoder type
0: Increment
1: Absolute
Note: Set whether use an absolute encoder by the bit 6 of parameter No.: 20.
3) Select the Max. allowable error
Note: System defaults 50.000mm, also, it can be set by data parameter P445.
4) Axis extensive card
0: Without extensive card
1: With extensive card
Note: Set whether use a bus servo card by the bit 6 of parameter No.: 0.
5) Grating type
0: Increment
1: Absolute
Note: Set whether use an absolute grating by the bit 0 of parameter No.: 1.
6) Spindle extensive card
0: Without extensive card
1: With extensive card
Note: Set whether the spindle drive is used the bus control method by the bit 1 of parameter No.: 1.
7) Multi-coil absolute zero setting
b) In the MDI mode, set the “Whether it is bus” to 1 in the bus configuration interface; set
c) Move the cursor to the
, press the <INPUT> twice based upon the prompts,
the zero return indicator is ON; the record of the motor absolute encoder along eac
axis at the current position is regarded as machine zero; the system is restarted after
the power is turned off, and the zero return indicator is still ON. Manually set the
negative/positive boundary based upon the Max. stroke of the actual machine tool,
so that move the current machine tool an offset value forward or backward, lastly,
the bit 6 of parameter No.: 61 is set to 1, the positive/negative is then enabled.
Setting
range:
-99999.9999~99999.9999,
alternatively,
the
positive/negative
boundary along with each axis can be directly set by data parameters P450~P459.
D) Whether configure the griding. Separatly set whether each axis is configured with a
griding, 0: Without, 1: With. Alternatively, individually set it by bit 3 and 7 of
parameter No.: 1.
4. Confirm it by
.
Note 1: After the machine tool zero is set, if the zero return direction, feed axis movement direction, servo and
system gear ratio of the system are altered, the zero will lost, and therefore, it is necessary to reset the zero of the
machine tool.
Note 2: After the machine tool zero is set, the other reference points may be affected, for example, the 2nd and
the the 3rd reference points should be set again.
233
VOLUME II
OPERATION
the “Encoder type” to 1; set the machine zero position moving each axis manually.
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3.3.5.1 Servo Parameter Display
Enter the servo debugging interface by pressing the【
servo parameter interface by the【
BUS CONFIGURATION】, then enter the
SERVO PARAMETER】. The content of this interface is shown
below (Fig. 3-3-5-1-1).
VOLUME II
OPERATION
Fig. 3-3-5-1-1
3.3.5.1.1
Modification & Setting of Servo Parameter
1) Select <MDI> operation mode.
2) Enter the <SETTING> interface by
3) Press the
, then the【
, set the parameter switch to “1”.
BUS CONFIGURATION】to enter the servo debugging
interface; enter the parameter setting and display screen by the【
SERVO PARAMETER】.
4) Move the cursor to the selected axis parameter #0; input the password 315 (Parameters 0~42
can be viewed or altered); download the drive to the system by input button; the servo
parameter can be modified in the【SERVO PARAMETER】interface.
5) Move the cursor to the position where the parameter number is to be modified:
Method 1: Display the page to be set a parameter by page up/down button; alternatively,
move the cursor by direction buttons to position the parameter position to be modified.
234
Chapter Three
Interface Display & Data Modification & Setting
Mehtod 2: Positioning is performed by
6) Confirm it by
after inputting a parameter number.
, the parameter value is delivered to drive, and the state column displays
“Successful for drive parameter download!”.
7) The servo saves the updated parameter by
, and the state column displays
“Successful for drive parameter save!”.
8) Close the parameter switch after the overall parameters setting are executed.
3.3.5.1.2
Matched Parameter Setting Between Servo & Motor Type
1) Select the <MDI> mode.
2) Enter <SETTING> interface by
, then enter to the servo debugging interface by 【
CONFIGURATION】, lastly, enter the parameter display page by【
BUS
SERVO PARAMETER】.
4) Move the cursor to the current selected axis parameter #0, input the password 385, download
the drive parameter to the system by input button, modify the servo parameter in the
【SERVO PARAMETER】interface.
5) Move the cursor to the parameter #1, input the matched numerical value to the motor type:
6) Confirm it by
, the parameter value is delivered to the drive, and the state column
displays “Successful for drive parameter download!”.
7) Servo saves the updated parameter by
, and the state column displays “Successful
for drive parameter save!”.
8) Close the parameter switch after the overall parameters setting are completed.
3.3.5.1.3
Servo Parameter Backup
1) Select the <MDI> operation mode.
2) Enter the <SETTING> interface by
, set the parameter switch to “1”.
235
VOLUME II
OPERATION
3) Firstly, press the
, set the parameter switch to “1”.
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3) Enter the <SETTING> interface by
, input the terminal user password or above.
, enter the servo debugging interface by【
4) Control the
BUS CONFIGURATION】,
SERVO PARAMETER】.
and then enter the parameter display screen by【
5) Select the【BACKUP】button, the parameter of the current selected axis is copied to the file
DrvParXX.txt. (XX axis number. For example: the file name is DrvPar01.txt if the X axis is
backup.)
6) Close the parameter switch after the overall parameters setting are completed.
3.3.5.1.4
Recovery of Servo Parameter
1) Select the <MDI> operation mode.
VOLUME II
OPERATION
2) Enter the <SETTING> interface by
, set the parameter switch to “1”.
3) Enter the <SETTING> interface by
, input the terminal user password or above.
4) Press the
, enter the servo debugging interface by【
then enter the parameter display screen by【
BUS CONFIGURATION】, and
SERVO PARAMETER】
5) Select the【RECOVERY】button, the backup file DrvParXX.txt of the current selected axis is
recovered to the servo drive. (XX axis number. For example: the file name is DrvPar01.txt if
the X axis is backup.)
7) Servo saves the updated parameter by
, and the state column displays “Successful
for drive parameter save!”.
7) Close the parameter switch after the overall parameters setting are completed.
3.3.5.1.5
Servo Level Zering
The machine tool trembles due to the excessive big of the servo parameter rigid when debugging
the parameter. To avoid the hazard, the servo parameter can be recovered into 0 level initial state
parameter by the function of the servo level zeroing.
1) Select the <MDI> operation mode.
2) Enter the <SETTING> interface by
236
, set the parameter switch to “1”.
Chapter Three
Interface Display & Data Modification & Setting
3) Enter the <SETTING> interface by
4) Press the
, input the terminal user password or above.
, enter the servo debugging interface by【
then enter the parameter display screen by【
BUS CONFIGURATION】, and
SERVO PARAMETER】
5) The overall servo axis parameters can be recovered into the parameter of the 0 level by the
button of【LEVEL ZEROING】.
7) Servo saves the updated parameter by
, and the state column displays “Successful
for drive parameter save!”.
7) Close the parameter switch after the overall parameters setting are completed.
3.3.5.2 Spindle Parameter
When the spindle drive is selected as bus control mode by the system (Bit 1 of parameter No.:1
sets to 1), user can check and set the corresponding servo drive parameters of the spindle in the
【SPINDLE PARAMETER】interface.
Spindle Parameter Display
When the bit 4 of parameter No.: 0 is set to 0, the system uses the single spindle control, enter
the spindle parameter interface by【SPINDLE PARAMETER】softkey. The content of this interface is
shown below (Refer to the Fig. 3-3-5-2-1-1).
Fig. 3-3-5-2-1-1
237
VOLUME II
OPERATION
3.3.5.2.1
GSK218MC Series Machining Center CNC System Programming & Operation Manual
When the bit 4 of parameter No.: 0 is set to 1, the system uses the double-spindle control, enter
the spindle parameter interface by【SPINDLE PARAMETER】softkey. The content of this interface is
shown below (Refer to the Fig. 3-3-5-2-1-2).
Fig. 3-3-5-2-1-2
VOLUME II
OPERATION
3.3.5.2.2
Modification and Setting of Spindle Parameter
1) Select the <MDI> operation mode.
2) Enter the <SETTING> interface by
4) Press the
, set the parameter switch to “1”.
, and then enter the parameter display screen by【
SPINDLE
PARAMETER】softkey.
4) Move the cursor to the selection axis parameter #0, input the password 315 (Parameters 0～
160 can be viewed and altered); download the drive parameter to the system by input button,
and the servo parameter can be modified by【SPINDLE PARAMETER】interface.
5) Move the cursor to the position where to be modified the parameter number:
Method 1: Display the page to be set the parameter by page up/down; or move the cursor by
direction buttons, and the position the parameter position where to be modified.
Method 2: Press the
to position after inputting the parameter number.
6) Input the new parameter value by numerical buttons (Modify the parameters with different
levels, and the password authority of the corresponding level should be input accordingly).
238
Chapter Three
7) Confirm it by
Interface Display & Data Modification & Setting
, the parameter value is then input, and the state column displays
“Successful for drive parameter download!”.
8) Servo saves the updated parameters by
, and the state column displays “Successful
for drive parameter save!”.
9) Close the parameter switch after the overall parameters setting are completed.
3.3.5.2.3
Backup of Spindle Parameter
1) Select the <MDI> operation mode.
2) Enter the <SETTING> interface by
, set the parameter switch to “1”.
3) Enter the <SETTING> interface by
, input the terminal user password or above.
, and then enter the parameter display screen by【
SPINDLE
PARAMETER】softkey.
5) Select the【BACKUP】button, the parameter of current selected axis can be copied to the file
DrvParXX.txt. (XX axis number. For example: the file name is SP01.txt if the X axis is
backup.)
6) Close the parameter switch after the overall parameters setting are completed.
3.3.5.2.4
Recovery of Spindle Parameter
1) Select the <MDI> operation mode.
2) Enter the <SETTING> interface by
, set the parameter switch to “1”.
3) Enter the <SETTING> interface by
, input the terminal user password or above.
4) Press the
, and then enter the parameter display screen by【
SPINDLE
PARAMETER】softkey.。
239
VOLUME II
OPERATION
4) Press the
GSK218MC Series Machining Center CNC System Programming & Operation Manual
5) Select the【RECOVERY】button, the backup parameter file SPXX.txt of current selected axis
can be recovered to the servo drive. (XX axis number. For example: the file name is
SP01.txt if the X axis is backup.)
6) Servo saves the updated parameter by
, and the state column displays “Successful
for drive parameter save!”.
7) Close the parameter switch after the overall parameters setting are completed.
3.3.5.3 Servo Debugging Tool STT
In order to guarantee that the servo debugging function is really reacted the servo capacity, it is
better to cancel the gear ratio at the drive side and each compensation (Including the pitch error
compensation and reverse interval compensation) at the system side.
3.3.5.3.1
Interface Composition
VOLUME II
OPERATION
Enter to the servo debugging tool interface by【 STT】. The content of this interface is as the Fig.
3-3-5-3-1~ 3-3-5-3-2).
Fig. 3-3-5-3-1 Rigid level interface
240
Chapter Three
Interface Display & Data Modification & Setting
Note: The coordinate axis display on the servo debugging interface is determined by the system
control axis numbers and the least number in the bus servo slave-station.
3.3.5.3.2
Function Introduction
1. Rigid grade and parameter optimization operation function
This function is for setting the servo parameter to the optimization state of the servo
performance.
2. Round testing
The round testing can be judged the response synchronism of each servo axis for the
machine tool by collecting the motor encoder position information based upon imitating the
round of the circle cutting movement.
3.3.5.3.3
Operation Explanation
1. Rigid grade debugging operation
Explanation: the debugging and setting of rigid grad, only one axis can be operated
once.
Operation buttons:
A.
and
buttons: Selection axis. (Note: The up/down direction buttons
241
VOLUME II
OPERATION
Fig. 3-3-5-3-2 Roundness measure interface
GSK218MC Series Machining Center CNC System Programming & Operation Manual
can not be changed the axis in the current operation once entering the optimization
schedule.)
B.
and
buttons: Reduce or increase the rigid grade of the current axis,
the rigid level reduces or increases one level by every one push;
C. 【AXIS SHIFTING+】and【AXIS SHIFTING -】softkeys: Move the current axis for a
distance positively or reversely based upon the velocity from the data parameter P393 of
which this distance is determined by data parameter P392. Check whether the motor is
vibrative or abnormal noisy by repeatedly controlling the 【AXIS SHIFTING+】and【AXIS
SHIFTING -】softkeys before entering the optimizing schedule; the motor’s character can not
be gained by pressing the【AXIS SHIFTING+】and【AXIS SHIFTING -】softkey movement
axes consecutively once entering the optimizing schedule.
Note 1: Press the【AXIS SHIFTING+】and【AXIS SHIFTING -】softkey movement axes and
collect the data after entering the optimizing schedule.
Note 2: Never attempt to change the data parameters P392 and P393 without the professionals;
otherwise, the optimization may not succeed.
VOLUME II
OPERATION
D.
button: Confirm the operation or enter the next step;
E.
button: Cancel some one operation or return to the previous operation;
F.
button: Reset operation, return to the initial operation step.
G.
button: Save operation, save the optimized parameter.
Operation schedule: refer to the following figure:
242
Chapter Three
Interface Display & Data Modification & Setting
Enter the rigid
grade adjustment
and optimization
interface
No, continue
adjusting the
grade by
direction buttons
No: Press【 】
Or【 】to adjust the
rigid grade
Step1: Press
【 】or【 】to
adjust the rigid
grade
Reset to the
initialization
operation by
<RESET>
Whether enters
to the next step
or not
YES
Yes, press the <INPUT> to
clear the optimization state
and the optimization can be
performed again after
initializing
The rigid grad.
Step2：Measure
the rigid grade by
【SHIFTING+】or
【SHIFTING-】
No, enter the
optimization
schedule by
<INPUT>
Whether it is
vibration or
abnormal noise.
No: Return to grade
Adjustment by
<CANCEL>,
Directly adjust or
measure
The rigid grace after
cancelling.
Yes, enter the optimization
schedule by <INPUT>
Whether it is
already
optimized.
VOLUME II
OPERATION
NO
Step3: Enter the
optimization
schedule
Whether
optimizes
Yes, perform the optimization by【AXIS SHIFTING+】OR【AXIS SHIFTING-】
Step4:
Optimization
completed
No, clear the optimization data
after pressing the <CANCEL>,
and then optimizing again.
Whether
download the
parameter
YES
Step5: Download
the parameter by
<INPUT>
NO
Whether the
download is
successful!
YES
Enter the step 0 after the
operation is performed; select the
next axis to be optimized by
up/down direction buttons.
243
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2. Round testing
Operation buttons:
A. Number buttons: Input each parameter numerical value;
B.
and
buttons: Parameter selection;
C.
and
buttons: Function selection (Collection and analysis);
D.
button: Input parameter value or confirm it, and then perform the operation;
E.
button: Clear the data and then reset to the initial state.
Parameter items:
A. Plane: Select the testing plane G17, G18 and G19;
B. CW/CCW circle: Select the circle direction G02, G03;
C. Sampling period: Set the sample period, it is necessary to set based upon the circle
radius and feedrate; the bigger the radius is, the longer the sample period is; the slower
VOLUME II
OPERATION
the feedrate is, the longer the sampling period is;
D. Feedrate: The movement speed when testing.
E. Amplification: The round analysis is the magnification of the error amplification.
Operation steps:
Step 1: Select the collection function by
or
button after each parameter
is set;
Step 2: Start the arc and collect the data by pressing the
analysis function by
Step 3: Start the analysis function by
or
, and then select the
after the collection is performed.
, and then output the roundness data and draw
the round error distribution figure; refer to the following drawing.
244
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-3-5-3-3-1
Note: Measure the synchronism situation of the current each feed axis by the roundness testing
tools after the rigid grade and parameter optimization function debugging are performed. The
roundness testing of each plane is within 6u which is regarded as the synchronism of current
each servo axis is better, the parameter debugging is successful accordingly.
The double-drive offset generates during the operation of the system; adjust some one axis for
the double-drive by the【DOUBLE-DRIVE DEBUGGING TOOL】; at last, adjust the double-drive
parallel by observing whether the motor feedback current of the double-drive is consistent (or perform
the parallelism).
3.3.5.4.1
Double-drive Function Setting
When using the【DOUBLE-DRIVE DEBUGGING TOOL】, the data parameter P380 should be set
to 1~3 (1: The 4th axis is synchronic with the X axis; 2: The 4th axis is synchronic with the Y axis; 3:
The 4th axis is synchronic with the Z axis); also, the bit 0 of parameter No.:0 should be set to 1,
which is treated as the bus transition method of the drive, and it is necessary to debug in the MPG
mode.
3.3.5.4.2
Enter to Double-drive Debugging Function
In the double-drive debugging tool interface, after the interface is selected by the
on the controllable panel, enter to the parameter page display by【
button
BUS CONFIGURATION】softkey,
245
VOLUME II
OPERATION
3.3.5.4 Double-drive Debugging Tool
GSK218MC Series Machining Center CNC System Programming & Operation Manual
and then enter the double-drive debugging tool interface after selecting the【DOUBLE-DRIVE TOOL】
again. Refer to the Fig. 3-3-5-4-2-1.
VOLUME II
OPERATION
Fig. 3-3-5-4-2-1
3.3.5.4.3
Operation Explanation
If the parallelism verification should be performed by double-drive tool, the following steps are
necessary:
1. Shift to the MPG mode by controllable panel;
2. The step length of the MPG is adjusted to 0.001;
3. Set the 【 CALIBRATION SWITCH 】 to 1, in this case, the synchronism axis does not
performed at the same; each axis can be adjusted by MPG movement;
4. The MPG movement can be performed based upon the【CURRENT OFFSET】
，when the
，the system may alarm, it may
MPG movement exceeds 1mm of 【VERIFICATION LENGTH】
be moved again after the resetting cancels an alarm.
5. Set the【VERIFICATION SWITCH】to 0, in this case, the double-drive synchronism is
enabled; judge the motor’s current feedback (Alternatively, open the parallelism) is parallel by
moving the double-drive manually. Repeated the above steps 1~4 till the verification is
performed.
246
Chapter Three
Interface Display & Data Modification & Setting
3.4 Setting Display
3.4.1 Setting Page
1. Enter the page
Enter the setting information display interface by
interface:【SETTING】，【
WORKPIECE COORDINATE】，【
; there are 5 sub-interface in this
CENTER TOOL-SETTING】,【
，check and modification can be performed by the corresponding software,
DATA】and【PASSWORD】
refer to the Fig. 3-4-1-1:
VOLUME II
OPERATION
Fig. 3-4-1-1
2. 【SETTING】interface operation explanation
Press the【SETTING】softkey, check its parameters after the interface is set in the Fig. 3-4-1-1, as
well, the corresponding parameter can be modified.
The operation methods and steps are shown below:
(a) Enter the <MDI> operation method;
(b) Move the cursor by up/down button to the item to be changed;
(c) Input 0 or 1 according to the following explanations, or modify it by the left or right key;
1) Parameter switch
0: Close the parameter swith
1: Open the parameter switch
When the parameter switch sets to “0”, the modification and setting of the system
parameter are prohibited, the system alarm (0100: Parameter write is enabled) cancels. When the
parameter switch sets to “1”, the system alarm occurs (0100: Parameter write is enabled). In this
247
GSK218MC Series Machining Center CNC System Programming & Operation Manual
case, the alarm (This operation is only enabled in a setting interface) can be cancelled by
+
buttons.
2) Program switch
0: Close the program switch
1: Open the program switch
When the program switch sets to “0”, the program editing is prohibited.
3) Keyboard selection
0：MC-H
1：MC-V
2：MC
3：MC-U1
Note: In any method, the keyboard selection can be also altered if the ESP button is controlled.
4) Input unit
Set whether the input unit of the program is metric or inch
0: Metric
1: Inch
5) I/O channel
User freely sets it based upon its requirements, for example, the channel sets to 2 if the
DNC machining is performed by U disk; the channel sets to 3 if DNC machining is performed by
VOLUME II
OPERATION
internet access.
0, 1: RS232 (0 selects the Xon/Xoff agreement, 1 selects Xmodem agreement)
2：USB
3：NET
6) Automatic series No.
0: When the program is input by keyboard in the editing mode, the system will not
automatically insert the sequence number.
1: When the program is input by keyboard in the editing mode, the system will
automatically insert the sequence number. The incremental values of the sequence
numbers among each block are set by data parameter P210.
7) Sequence number increment
The incremental value when the automatic sequence number insertion is set, its range
is 0~1000.
8) Stop sequence number
This function can be set some one program that performs the single block dwell to the
specified block, which can be enabled when the program number and the block sequence
number are specified at the same time. For example: 00060 (Program number) is program
number O00060; 00100 (Sequence number) is block number N00100.
Note: When the stop sequence number is automatically set to -1 after the program operates to
the object block, and the single block dwell will not perform.
9) Date and time
User can set the system data and time at this position.
248
Chapter Three
(d) Control the
Interface Display & Data Modification & Setting
to input.
3.4.2 Workpiece Coordinate Setting Page
1. Enter the coordinate system setting interface by【
WORKPIECE COORDINATE】，the
content of this page is shown below (Fig. 3-4-2-1 ).
Additionally, there are 50 addition workpiece coordinate systems can be used other than 6
standard workpiece coordinate systems (G54～ G59). Refer to the Fig. 3-4-2-2. Each coordinate
system can be checked or altered by page up/down button. The operation of the additional
coordinate system, refer to the Section 4.2.9
Additional Workpiece Coordinate System in
PROGRAMMING.
Fig. 3-4-2-2
249
VOLUME II
OPERATION
Fig. 3-4-2-1
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2. There are two methods of coordinate input:
1) After entering this interface in any mode, move the cursor to the coordinate system to be
changed, and press the axis name from the desired setting value, and then confirm it by
; the value of the current machine coordinate system sets to the origin of the G
or ”X0”, and then
coordinate system, for example: press “X”, then
again.
The system may then automatically input the X axis machine coordinate of this point; in
addition, for example, input X10(X-10), then press the
, it means the X machine tool
coordinate value is +10(-10).
2) After entering this interface in any mode, move the cursor to the coordinate system axis to be
changed, directly input the machine tool coordinate value of the origin of the workpiece
coordinate system, and then confirm it by
.
VOLUME II
OPERATION
3) After entering this interface in any mode, move the cursor to the coordinate system axis to be
changed, directly input the machine tool coordinate value of the origin of the workpiece
coordinate system, and then confirm it by <INPUT>. In addition, press the softkey
<+INPUT> after the coordinate value is input, the system may automatically calculate the
new coordinate value and then display it.
3. The method of coordinate system search:
1) In any mode, press
to position after the coordinate system is input. For example:
input “G56”.
2) In any mode, for example, input “P6” or “P06”, press the
, the cursor will position at
the additional workpiece coordinate system “G54 P06”.
3.4.3 Center and Tool-setting Function
Enter the center and tool-setting function by【
CENTER TOOL-SETTING】
，the content of this
interface displays in the following figure (Refer to the Fig. 3-4-3-1 ).
250
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-4-3-1
3.4.3.1 Center Function Introduction & Operation Explanation
external circle, boss or groove can be performed the center measurement by the
Manual mode; the hole or external circle, boos or groove, vector hole or external,
vector boss or groove can be executed center measurement by Auto mode.
I. Manual Center
‹
Interface display
A. Hole or external circle
Fig. 3-4-3-1-1
B. Boss or groove
251
VOLUME II
OPERATION
Center measure: There are two center measurements: Manual and Auto. Wherein, only the hole or
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-4-3-1-2
‹
Manual center operations:
A. Option explanation:
VOLUME II
OPERATION
1. Measurement method:
0: Manual
1: Auto
2. Workpiece type:
1: Hole or external circle
2: Boss or groove
3. Coordinate system selection S:
G54~G59
G54 P1~P50
Set the center to the desired coordinate system after the
measurement is completed.
4. Measure point:
A. When the workpiece type is hole or external circle: there are 3 measurement points
(P1~P3), and the measurement will perform without particular order; wherein, if there are
3 points are overlapped, one of the point is regarded as the center coordinate; if there are
3 points are shared with a same straight line, the center coordinate can not be calculated,
and it is necessary to measure one of the point or the overall points again;
B. When the workpiece type is boss or groove: there are 4 measurement points (P1~P4),
and the measurement will perform without particular order; wherein, P1 and P2 are
separately two points along the X axis direction; P3 and P4 are separately two points
along the Y axis direction. The center coordinate of X axis direction calculates of the X
coordinate of P1 and P2; the center coordinate calculates of the Y coordinate of P3 and
P4.
B. Operation steps:
252
Chapter Three
Interface Display & Data Modification & Setting
Step 1: Press the <MEASURE> softkey after manually moving the tool or center bar to the 1st
measurement point.
Step 2: Repeated the step 1 till the overall measurement points are completed (There are 3
points for circle, and 4 points for rectangle).
Step 3: Set the center coordinate to the selected coordinate system by <START> softkey.
II.
Auto center
‹
Interface display and parameter option explanation
A. Public parameter option
1. Measurement method:
0: Manual
1: Auto
2. Workpiece type:
±1: Hole & external circle
±2: Boss & groove
±3: Vector hole & external circle
±4:
Vector boss & groove
【Note】-1: hole
+1: external circle
vector external circle
-2: groove
-4: vector groove
+2: Boss
-3: vector hole
+3:
+4: vector boss.
VOLUME II
OPERATION
3. Coordinate system selection S:
G54~G59
G54 P1~P50
4. Tool offset number T:
Tool offset number. The radius compensation value of the tool when the interpolation
machining is stored within the tool offset number.
5. Experience value tool offset number E:
The tool offset number is already registered the experience value. E and T will not assign
the same value when programming.
6. Rough center coordinate Cx:
The absolute coordinate value of the rouch center of the workpiece along X axis. If the
current point is set to rough center, directly press <INPUT> key to input a null value.
7. Rough center coordinate Cy:
The absolute coordinate value of the rouch center of the workpiece along Y axis. If the
current point is set to rough center, directly press <INPUT> key to input a null value.
8. Measure point coordinate Z:
The absolute position of the Z axis during measuring. If the current point is the
measurement point, directly press <INPUT> key to input a null value.
9. Profile dimension tolerance H:
253
GSK218MC Series Machining Center CNC System Programming & Operation Manual
The measured profile dimension tolerance value.
10. Radial interval R:
When measuring the external profile, the probe head is the distance from the destination
surface before the Z axis moves. The default is 8mm(0.3149inch) when the power is turned on.
11. Measure head overtravel distance Q:
The overtravel value of the measure head. Input a value by programming, the measure
head that uses this value to find a surface is regarded as the extra distance by exceeding
the destination dimension. If there is no programming, the default value is 10.0 mm (0.394
inch).
B. Hole & external circle parameter
VOLUME II
OPERATION
Fig. 3-4-3-1-3
1. Destination dimension D:
The Hole or diameter of the external circle to be measured. This value can not be a null or 0.
C. Boss & groove parameter
254
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-4-3-1-4
1. Destination dimension Lx:
The profile dimension along X axis direction to be measure. The measurement along
2. Destination dimension Ly:
The profile dimension along Y axis direction to be measure. The measurement along
this axis can not be performed when this parameter option is null or 0.
【Note】: Lx and Ly can not be set to null or 0 at the same time.
D. Vector hole & external circle
Fig. 3-4-3-1-5
255
VOLUME II
OPERATION
this axis can not be performed when this parameter option is null or 0.
GSK218MC Series Machining Center CNC System Programming & Operation Manual
1. Destination dimension D:
The diameter of the hole or external circle to be measured. This value can not be set to
null or 0.
2. Start angle A:
The angle by the 1st vector measure, calculate from the X+ direction. If it is ignored, the
alarm issues.
3. The 2nd angle B:
The angle of the 2nd vector measure, calculate from the X+ direction. If it is ignored, the
alarm issues.
4. The 3rd angle C:
The angle of the 3rd vector measure, calculate from the X+ direction. If it is ignored, the
alarm issues.
【Note】The least D-value between any two point angle is determined by “#5=
” in
program O09729, the default is 5. If the least D-value should be changed, modify
the “#5=
”.
VOLUME II
OPERATION
E. Vector boss & groove
Fig. 3-4-3-1-6
1. Destination dimension D:
The profile diemension to be measured. The measurement of this axial will not perform
when the parameter is null or 0.
256
Chapter Three
Interface Display & Data Modification & Setting
2. Start angle A:
Measured plane calculates the angle from the X+ direction.
‹
Data input
A. The condition of the data input
When the Auto center measurement does not start, the data can be input in any operation
method.
B. Input format
1. Data +<INPUT> inputs the desired data;
2. Directly control the <INPUT> button to enter the null value;
3. When the current line is the rough center coordinate X, rough center coordinate Y,
measurement point coordinate Z, the following formats can be input:
① Directly input null value by <INPUT>;
② X/Y/Z+ <INPUT> input the current absolute coordinate value;
③ X/Y/Z+ data + <INPUT> input the current absolute coordinate value of the selected
axis + data.
④ Directly press the [MEASURE] software to input the absolute coordinate value of
⑤ X/Y/Z+ [MEASURE] input the absolute coordinate value of current axis;
⑥ X/Y/Z+ data + [MEASUREMENT] input the current absolute coordinate value of the
selected axis + data;
‹
Operation steps:
Step 1: Set the center parameters of each item by turn;
Step 2: Shift to the Auto Mode.
Step 3: Start the automatic center program by <START>softkey, then measure the macro
program by <CYCLE START> button; the system will automatically set the center
coordinate to the selected workpiece coordinate system after the measurement is
performed.
3.4.3.2 Introduction and Operation Explanation of Tool-setting Function
‹
Interface display and function introduction
257
VOLUME II
OPERATION
current axis;
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-4-3-2-1
Tool-setting function contains of the Auto tool length measurement and Z axis workpiece
origin setting.
A. Tool measurement:
VOLUME II
OPERATION
Auto tool length measurement is performed the measurement to the different tool length and
dirameter by the tool-setter which is installed on the workpiece. The length and diameter of each
tool is automatically set to the specified tool offset register, so that the tool can be correctly
machined even if the different length and diameter are used at the same program.
B. The setting of the coordinate origin along the Z axis:
After the tool length measurement is completed, move the tool to the workpiece surface, in
this case, in this case, the current machine coordinate value that is regarded as the origin sets to
the
selected
workpiece
coordinate
(G54~G59
G54
P1~P50)
by
pressing
<MEASUREMENT> softkey.
‹
Tool measurement
A. Parameter option explanation
1. Measurement mode selection:
1: Length
2: Diameter 3: Length & Diameter calibration
4: Length calibration
2. Tool number T:
The current tool number to be measured.
3. Tool length offset number H:
Store the offset number of the current tool length (It’s default is same with the T).
4. Cutter diameter offset number D:
258
the
Chapter Three
Interface Display & Data Modification & Setting
Store the offset number of the current tool diameter (It’s default is same with the T).
5. Cutter diameter S:
The diameter for the measured tool, when S is “+” value that means the tool is the
right-handed direction cutting; when S is “-“ value that means the tool is the left-handed direction
cutting. When the cutter radius offset No. D in the register is already treated as the nominal tool
diameter, the value may not be input. (This parameter value is cleared after the tool No. T is
altered.)
6. Tool length estimated measurement L:
The tool length is being measured. When the tool length offset No. H in the registered
is already regarded as the nominal tool length, the value may not be input. (This
parameter value is cleared after the tool No. T is altered.)
【Note 1】: When the measurement mode is selected as the length carlibration, this
length should be input and regarded as the standard tool (Refer to the mandrel)
length.
7. Measurement depth Z:
value –5.0mm [–0.20 inch]), negative value means the downward.
8 Overtravel value R&Q:
The overtravel value and the radial interval moving to the prober side downward.
(Default value 4.0 mm [0.16 inch]).
【 Note 2 】 It is the overtravel value along the length direction when the length
measurement is performed; it is the radial overtravel value in the diameter
measurement; and the overtravel value along the length direction and the radial
overtravel value are same when the length & diameter measurement are executed.
9. Worn mark tool offset number:
A null tool offset number is used as the position of the tool wore mark.
10. Wore allowrance tolerance I:
Cutter dimension adjustment compensates the cutting state of the tool. The positive
value brings that the actual radius is less than the specified value, for example I=.01
means that the tool radius is less than 0.01. Also, set the nominal cutter radius value
to 0 by input its value.
【Note 3】：It is used for setting the tool-setting prober diameter when the diameter
calibration is executed.
B. Measurement parameter inputs the operation steps:
1. The selection of item: it can be selected by moving the cursopr up/down button.
259
VOLUME II
OPERATION
The depth from the prober surface to the diameter measurement position (Default
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2. Data input: Whn the Auto tool measurement does not start, in any operation mode,
input the data, then the ENTER, and the each data can be modified accordingly.
C. Operation steps:
Step 1: Set each tool measurement parameter in turn
Step 2: Shift to the Auto mode.
Step 3: Start the automatic tool-setting main program by <START> softkey, then operate
the macro program measurement by <CYCLE START>again; automatically
specifiy the tool length and radius write-in to the offset registered.
‹
Workpiece origin setting along Z axis
Notice: Ensure that the current tool is already performed the automatic tool
measurement before the Z axis workpiece origin is set; otherwise, the machining error
may occur, and the tool and equipment may be damaged, as well the personnel safety.
A. The selection of the coordinate system:
1. Setting range: G54~G59
G54 P1~P50
2. Data input: When the automatic tool measurement does not start, in any operation
mode, move the cursor to the coordinate system option, and then input the data based
VOLUME II
OPERATION
upon the following formats:
a. The integer of 54~59
b. G54~G59；
c. P1~P50. Then press the<INPUT> button。
B. The setting of the workpiece origin:
1. Setting range: -9999.999~9999.999
2. Data input: When the automatic tool length measurement does not start, in any
operation mode, move the cursor to the coordinate system selection option, set the
current Z axis moachine coordinate value to the Z axis of the current selected workpiece
coordinate system by directly pressing the [MEASUREMENT] software, alternatively,
input the data based upon the following formats:
a. Input format: Z;
b. Z+ data; Set the current machine coordinate value along Z axis + the
input data to the Z axis of the current selected workpiece coordinate
system by [MEASUREMENT] softkey accordingly.
3.4.4 Backup, Recovery and Transmission of Data
Enter the setting (Data treatement) interface by【
DATA】. The user data (Ladder diagram,
ladder diagram parameter, system parameter value, tool compensation value, pitch compensation
260
Chapter Three
Interface Display & Data Modification & Setting
value, system macro variable, user macro program and CNC component program) can perform both
the backup (save) and recovery (read) and the data output and input operations by U disk or PC
machine. Simultaneously, the data back and recovery are performed, the component program
memoried in the CNC will be regardless.
Fig. 3-4-4-1
1. Set the corresponding level password in the password interface by【PASSWORD】
softkey. Refer to the Setting and Modification of Password Authority in the Section 3.4.5
for the corresponding password level of each data operation.
2. Enter the data treatment operation interface by【
DATA】twice, refer to the Fig.
3-4-4-2.
Fig. 3-4-4-2
261
VOLUME II
OPERATION
Operation method:
GSK218MC Series Machining Center CNC System Programming & Operation Manual
by 【X】.
Enter the next page
The function of each operation items are shown below: (Table 3-4-4-1)
Table 3-4-4-1
Operation
Function Explanation
Item
Separatly perform the data backup, such as the ladder diagram
(PLC),
Data backup
parameter
(PLC),
system
parameter
value,
cutter
compensation value, pitch compensation value and system macro
variable etc. in the system disk. The system will generate .bak backup
file after the data backup is executed.
Separatly perform the data recovery, such as the ladder diagram
(PLC),
Data recovery
parameter
(PLC),
system
parameter
value,
cutter
compensation value, pitch compensation value and system macro
variable etc. in the system disk. The system recovery operation is
read and recovered the backup file from system.
VOLUME II
OPERATION
Data output
Data input
One-Touch
backup
One-Touch
recovery
One-Touch
output
One-Touch
input
The data output operation can be output the data in the system disc to
the external storage device.
The data input operation can be input the data in the external storage
device to the system disc.
Simultaneously backup the multiplication data to the system disk.
Simultaneously recover th+e backup file for the multiplication data
items
Simutaneously copy the file for the multiplication data items in the
system disk to the U disk.
Simultaneously copy the multiplication file in the U disk to the
corresponding data item in the system disk.
3. Select the destination file by
file list table by
or
or
direction button; Shift the data item list and
.
4. The operations, such as the data backup, data recovery, data output, data input, one-touch
backup, one-touch recovery, one-touch output and one-touch input, are performed by its
corresponding softkey.
Note:
1) The softkey functions both the data output and the data input are consistent when I/O channel sets to
262
Chapter Three
Interface Display & Data Modification & Setting
U disk.
2) For the output/input operation of the data, guarantee the the correctly set of the I/O channel. The I/O
channel should be set to 0 when using U disk; I/O channel should be set to 0 or 1 when using the
transmission software by PC machine.
3) The content of one-touch operation is determined by password authority; refer to the Section 3.4.5 of
OPERATION EXPLANATION for the corresponding relationships between the each data item and
password authority.
4) Relevant parameter:
① It is set by the bit 7 of parameter No.: 54: Whether the one-touch input/output
② It is set by bit 0 of parameter No.:27: Whether forbid the subprogram editing of program numbers
80000-89999.
③ It is set by bit 4 of parameter No.:27: Whether forbid the subprogram editing of program numbers
90000-99999.
5) During the treatment of the data, the system sets a relevant opration prompt, its prompt
content shows below: (Table 3-4-4-2).
Table 3-4-4-2
Series
Prompt Information
No.
1
Reason
One-touch operation completion
Successful operation
system prompts: The copy can be
performed after the parameter is
altered.
3
The input/output operation
of the macro program is
performed, however the
relevant parameter of the
The system alarm after one-touch
The ladder diagram and
operation
The
the parameter update of
parameter that should be cut off
the ladder diagram are
the
performed, it is better to
is
primary
completed:
power-source
is
power on again.
4
Fail to read the file
File error
5
Fail to write the file
File error
6
Fail to copy the file
File error
File excessive big, it is better to
Component
use DNC
more than 4M
The remainder space is absent
Adequate space
8
Skip
the
input/output
operation of this file.
system does not set.
modified.
7
Transmission completion
The
transmission
executed,
should
be
the
is
power
turned
on
again.
Interrupt
input/output
operation
Interrupt
input/output
operation
Interrupt
input/output
operation
program
is
Interrupt
input/output
operation
Interrupt
input/output
operation
6) The LADCHI**.TXT file is disabled after transiting the system, which can be enabled after the power is
turned on again.
263
VOLUME II
OPERATION
One-touch operation completion,
2
Troubleshooting
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3.4.5 Setting & Modification of Password Authority
GSK218MC system provides authority setting function to avoid the machining program or CNC
parameter is maliciously modified; password divides into 5 levels: the 1st level (System factory), the
2nd level (Machine tool factory), the 3rd level (System debugging level), the 4th level (Terminal user)
and the 5th level (Machining operation) based upon the high-to-low. The default is lowest leve when
the machine’s power is turned on (Refer to the Fig. 3-4-5-1).
The 1st level, 2nd level: The state parameter, data parameter, cutter compensation parameter and
the transmission PLC ladder diagram, etc. of the CNC can be modified.
The 3rd level: The state parameter, data parameter and cutter compensation data and pitch
compensation, etc. of the CNC can be modified.
The 4th level: The state parameter, data parameter of partial CNC can be modified.
The 5th level: Without password level. It can be both modified the cutter compensation data,
macro program and performed the machine tool operation panel, instead of altering the state
parameter, data parameter and pitch compensation data of the CNC.
VOLUME II
OPERATION
Fig. 3-4-5-1
1) After entering this interface by <MDI MODE>, position to the destination position by moving
the cursor.
2) Input the password of the corresponding level, then press the
, if it corrects, the
system will prompt “Password Correct”.
3) Input the digits 0~6 or letters when the system passwords are modified, then press the
to confirm it.
264
Chapter Three
4) Press the
Interface Display & Data Modification & Setting
key after altering, cursor moves to the “CANCEL (END)” button, the
interface prompts: “Press <INPUT> button to confirm the cancel!”. After controlling the
, the interface prompts: “Cancel completion!”, simultaneously, cursor returns to the
password setting column. The password will be automatically cancelled after the power is
turned off till to the reatart is performed.
3.5 Figure Display
Enter the figure page by
. There are two display interfaces【FIGURE PARAMETER】and
【 FIGURE】，which can be displayed by its corresponding softkey. Refer to the following figure (Fig.
3-5-1):
VOLUME II
OPERATION
Fig. 3-5-1
1) Figure parameter interface
Enter the figure interface by【FIGURE PARAMETER】，refer to the Fig.
3-5-1.
A. The meaning of the figure parameter:
Coordinate selection: Set the drawing plane, there are 6 methods (0~5), for example, the
2nd line shows.
Figure mode: Set the figure display mode.
Auto erasion: When it is set to 1, the program figure is automatically erased at the next
circular start performed till to the program is ended.
Scaling: Set the proportion of the drawing.
Figure center: Set the corresponding workpiece coordinate value of the LCD based upon
265
GSK218MC Series Machining Center CNC System Programming & Operation Manual
the workpiece coordinate.
The Max./Min. value: After the Max./Min. value of the display axis is set, the CNC system
may automatically set the scaling proportion or figure center value.
The Max. value of X: The Max. value along X in figure display (Unit: 0.0001mm /
0.0001inch)
The Min. value of Y: The MIN. value along Y in figure display (Unit: 0.0001mm / 0.0001inch)
The Max. value of Y: The Max. value along Y in figure display (Unit: 0.0001mm /
0.0001inch)
The Min. value of Y: The Min. value along Y in figure display (Unit: 0.0001mm / 0.0001inch)
The Max. value of Z: The Max. value along Z in figure display (Unit: 0.0001mm /
0.0001inch)
The Min. value of Z: The Max. value along Z in figure display (Unit: 0.0001mm / 0.0001inch)
B. The setting method of figure parameter:
a. Move the cursor under the set parameter;
b. Input the corresponding numerical value based upon the actual requirement;
c. Confirm it by
VOLUME II
OPERATION
2) Figure interface
.
Enter the interface interface by【 FIGURE】. (Refer to Fig. 3-5-2):
Fig. 3-5-2
The machining path of the operated program can be monitored in the figure page.
A. Enter to the drawing state by【START】or
, in this case, ‘*’ moves to S: Before the
drawing start;
B. Enter the stop drawing state by【STOP】or
266
, in this case, ‘*’ moves to T: Before the
Chapter Three
Interface Display & Data Modification & Setting
drawing stop;
C. The figure shifts in the corresponding figures 0～5 by pressing【SHIFT】every time.
D. Clear the drawn figure by【Clear】or
.
3.6 Diagnosis Display
The state of DI/DO signal between the CNC and machine tool, the signal state for transmitting
between the CNC and PLC, and the PLC internal data and CNC internal state are displayed on the
diagnosis page. The corresponding meanings and setting methods for each diagnosis number are
shown the GSK 218MC CNC System PLC & Installation Connection Manual.
This diagnosis uses for detecting the CNC interface signal and internal signal operation state,
which can not be modified.
Enter the diagnosis display interface by
; there are 5 sub-interface in this page:
corresponding software (Refer to the Fig. 3-6-1).
Fig. 3-6-1
267
VOLUME II
OPERATION
【 SIGNAL】，
【SYSTEM】
，【BUS】
，【DSP】and【 FLUCTUATION】, which can be viewed by its
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3.6.1 Diagnosis Data Display
3.6.1.1 Signal Parameter Display
Enter the signal diagnosis interface by【SIGNAL】softkey. The content of this interface is shown
below (Refer to the Fig. 3-6-1-1-1~Fig.3-6-1-1-4).
1. F signal interface
Enter the diagnosis (NC→PLC) interface by 【 F SIGNAL 】 in the
<DIAGNOSIS> interface. Refer to the Fig. 3-6-1-1-1.
VOLUME II
OPERATION
Fig. 3-6-1-1-1
This signal is delivered to PLC from system, its meanings and setting methods of each diagnosis
number are shown in the matched GSK 218MC CNC System PLC & Installation Connection Manual.
2. G signal interface
Enter the diagnosis (PLC→NC) interface by【G SIGNAL】softky in the
<DIAGNOSIS> interface. Refer to the Fig. 3-6-1-1-2:
Fig. 3-6-1-1-2
268
Chapter Three
Interface Display & Data Modification & Setting
This signal is delivered to PLC from system, its meanings and setting methods of each diagnosis
number are shown in the matched GSK 218MC CNC System PLC & Installation Connection Manual.
3. X signal interface
Enter the diagnosis (MT→PLC) interface by【X SIGNAL】softkey in the
<DIAGNOSIS> interface. Refer to the Fig. 3-6-1-1-3:
Fig. 3-6-1-1-3
number are shown in the matched GSK 218MC CNC System PLC & Installation Connection Manual.
4. Y signal interface
Enter the diagnosis (PLC→MT) interface by【Y SIGNAL】softkey in the
<DIAGNOSIS> interface. Refer to the Fig. 3-6-1-1-4:
Fig. 3-6-1-1-4
This signal is delivered to PLC from system, its meanings and setting methods of each diagnosis
number are shown in the matched GSK 218MC CNC System PLC & Installation Connection
Manual.
269
VOLUME II
OPERATION
This signal is delivered to PLC from system, its meanings and setting methods of each diagnosis
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3.6.1.2 System Parameter Display
Enter the system signal diagnosis interface by【SYSTEM】softkey. The content of this interface is
shown below (Refer to Fig. 3-6-1-2-1).
Fig. 3-6-1-2-1
VOLUME II
OPERATION
3.6.1.3 Bus Parameter Display
Enter the bus signal diagnosis interface by【BUS】. The content of this page is shown below
(Refer to the Fig. 3-6-1-3-1).
Fig. 3-6-1-3-1
270
Chapter Three
Interface Display & Data Modification & Setting
3.6.1.4 DSP Parameter Display
Enter the bus signal diagnosis interface by【DSP】. The content of this page is shown below
(Refer to the Fig. 3-6-1-4-1).
Fig. 3-6-1-4-1
VOLUME II
OPERATION
3.6.1.5 Fluctuation Parameter Display
Enter the fluctuation interface by【FLUCTUATION】softkey. Refer to the Fig. 3-6-1-5-1:
Fig. 3-6-1-5-1
271
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Axis selection: Select the axis to be performed the fluctuation diaganosis.
Fluctuation selection: Select the content of the diagnosed fluctuation.
Proportion of horizontal axis, vertical axis: Select the drawn proportion
Data: In any mode, input the corresponding data, then confirm it by
.
Signal monitoring performs by <START> button, and stop it by <STOP> button.
3.6.2 Check Signal State
1) Select the corresponding display interface by
.
2) The corresponding address explanation and meaning at the lower left of the screen when
moving the cursor left or right.
3) You can find the destination address by moving the cursor or input the desired search
VOLUME II
OPERATION
parameter address, then control the
button.
4) 【 FLUCTUATION 】 interface can be displayed the velocity, acceleration and addition
acceleration for debugging, and then find the optimized adapted parameter of the drive and
motor.
3.7 Alarm Display
The “alarm” information displays at the lower-left-corner on the screen when the system alarm
issues. In this case, the display page appear by
. There are four display interfaces in this
【
, USER】
【
, HISTORY】
【
, RECORD】, which can be checked (Refer to the Fig. 3-7-1～
page:【ALARM】
Fig.3-7-4) by its corresponding softkey. Alternatively, whether shifting to the alarm interface when bit 6
of parameter No.: 24 alarm occurs.
1. Alarm interface
the Fig. 3-7-1:
272
Enter the alarm interface by【ALARM】softkey in <ALARM> interface, refer to
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-7-1
Display the detailed content of the current P/S alarm number on the alarm display screen. Refer
to the appendix two for the detailed alarm content.
2. User interface
Enter the external alarm interface by【USER】softkey in <ALARM> interface, refer
VOLUME II
OPERATION
to the Fig. 3-7-2:
Fig. 3-7-2
The detailed content of each user alarm information shows in the GSK 218MC CNC System PLC &
Installation Connection Manual.
Note: The external alarm can be set and edited the alarm number based upon the on-site actual circumstance
by the user, and the alarm content after edited inputs to the system by the system transmission
software. The external alarm is the A of the edited file LadChi**.txt, the followed two-digit are set by the
273
GSK218MC Series Machining Center CNC System Programming & Operation Manual
value of the bit parameters 53.0~53.3. (Default vaue is 01, that is, the file name is LadChi01.txt).
3. History interface
Enter the history alarm information interface by【HISTORY】softkey in <ALARM>
interface, refer to the Fig. 3-7-3:
Fig. 3-7-3
This items within this interface are arranged from near to far based upon the time sequence, so
VOLUME II
OPERATION
that the user can easily view it.
4. Record interface
Enter the external alarm interface by【RECORD】softkey in <ALARM> interface,
refer to the Fig. 3-7-4:
The content of operation record interface is the concrete modification information for the system
parameter and ladder diagram, such as the modification content and time, etc.
Fig. 3-7-4
Operation record can be display 34 pages, and history alarm information can be shown 9 pages,
such as, the alarm time, alarm number, alarm information, page, etc. which can be viewed by page
up/down button.
274
Chapter Three
Interface Display & Data Modification & Setting
The record of history and record can be deleted (The password level is the debugging or more
than the debugging level) by
button.
3.8 Program-Control Display
Enter the program-control display page by
, and there are 5 display interfaces in the
，
【 PLCGRA】，
【 PLCPAR】，
【PLCDGN】and【 PLCTRACE】, which can be shifted
page:【INFO】
by the corresponding softkey. The concrete content is shown below (Refer to the Fig. 3-8-1～3-8-5).
VOLUME II
OPERATION
Fig. 3-8-1
Fig. 3-8-2
275
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
Fig. 3-8-3
Fig. 3-8-4
276
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-8-5
The modification methods and relevant information for the PLC ladder diagram are shown in the GSK
218MC CNC System PLC & Installation Connection Manual.
Enter the help display page by
, there are eight display interfaces in this page:【SYSTEM
【OPERATION TABLE】
【ALARM TABLE】
【G CODE TABLE】
【PARAMETER TABLE】
INFORMATION】
【 PLC.AD】
【COUNTER】, which can be viewed by its corresponding softkey.
【MACRO COMMAND】
The displayed content shows below (Refer to Fig. 3- 9- 1～3- 9- 12).
1. System information interface
Enter the system information interface by 【 SYSTEM
INFORMATION】softkey in <HELP> interface; refer to the Fig. 3-9-1:
Fig. 3-9-1
277
VOLUME II
OPERATION
3.9 Help Display
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2. Operation table interface
Enter the help information (Operation list) page by【OPERATION
TABLE】softkey in <HELP> interface; refer to the Fig. 3-9-2:
Fig. 3-9-2
In the help information (Operation list) interface, the operation steps and methods in each
VOLUME II
OPERATION
interface are detailed. The unfamiliar or unclear operations can be searched and compared in the
help interface.
3. Alarm table interface Enter the help information (Alarm list) page by【ALARM TABLE】softkey in
<HELP> interface; refer to the Fig. 3-9-3:
Fig. 3-9-3
The meanings and troubleshootings in this interface are detailed.
4. G code table interface
Enter the help information (G code list) page by【G CODE TABLE】softkey
in <HELP> interface; refer to the Fig. 3-9-4:
278
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-9-4
The definition of each G code used by the system is introduced in G code interface, select the G
code to be check by cursor, and the G code definition shows at the lower-left-corner of the interface.
Refer to the Fig. 3-9-4. If you want to know the concrete format and usage of the G code, press the
; refer to the Fig. 3-9-5:
Fig. 3-9-5
The format, function, explanation and restriction of the code are detailed in this interface, as for
the unfamiliar or unclear code can be searched and compared in this page.
5. Operation table interface
Enter the help information (Parameter/Diagnosis table) page by
【PARAMETER TABLE】softkey in <HELP> interface; refer to the Fig. 3-9-6:
279
VOLUME II
OPERATION
on the panel after selecting the G code, and then return by
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-9-6
The parameter setting of each function is detailed in this interface, the unfamiliar or unclear
parameter setting can be searched and compared in the interface.
6. Macro command interface
Enter the help information (Macro command list) page by【MACRO
COMMAND LIST】softkey in <HELP> interface; refer to the Fig. 3-9-7:
VOLUME II
OPERATION
Fig. 3-9-7
The formats of macro commands and each operation code are introduced in this interface, and
the setting range of the local variable, universal variable and the system variable are provided. As for
the unfamiliar or unclear macro command operations can be searched and compared in the interface.
7. PLC.AD interface
Enter the help information (PLC address list) page by【PLC.AD】softkey in
，
【G ADDRESS】，
【X ADDRESS】 and
<HELP> interface. There are four sub-interface【F ADDRESS】
【Y ADDRESS】for the PLC address interface. The content shows below (Refer to the Fig. 3-9-8～
3-9-11).
280
Chapter Three
Interface Display & Data Modification & Setting
Fig. 3-9-8
VOLUME II
OPERATION
Fig. 3-9-9
Fig. 3-9-10
281
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 3-9-11
The address, symbol and meaning of the PLC are detailed in the PLC address interface, the
unfamiliar or unclear PLC addresses can be searched and compared in this page.
8. Counter interface
Enter the counter information page by【COUNTER】softkey in <HELP>
VOLUME II
OPERATION
interface; refer to the Fig. 3-9-12:
Fig. 3-9-12
In this page, the system provides the operation formats in this interface, such as the addition,
subtraction, multiplication, devision, sine, cosine and extraction, move the cursor positioning to the
space to be intput the data, and then input the data, then confirm it by
; the system may
automatically calculate the result after the desired data are input to the space followed the “=”.
282
Chapter Three
Pressing the
Interface Display & Data Modification & Setting
can be input the data again to calculate, the overall data in this interface are
then cleared.
VOLUME II
OPERATION
283
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
284
Chapter Four Manual Operation
CHAPTER FOUR
Enter the manual operation mode by
MANUAL OPERATION
, which contains of the manual feed, spindle control
and machine panel control, etc.
4.1 Coordinate Axis Movement
In the manual operation mode, each axis can be separately performed by the manual feedrate or
manual rapid traverse rate.
4.1.1 Manual Feed
or
, the corresponding axis
begins moving, and its movement speed can be changed by adjusting the feedrate; the axis
movement stops after releasing the button; the same as the Y axis and Z axis. This system,
temporarily, does not support the multi-axis movement at the same time, instead of the simultaneous
zero return along each axis.
Note: The manual feedrate of each axis is set by parameter P98.
4.1.2 Manual Rapid Traverse
Press the
, the indicator is on, then enter the manual rapid traverse state, and then
each axis operates at the rapid traverse rate pressing the button of the feed direction axis.
Note 1: The manual rapid traverse rate is set by P170~ P173.
Note 2: The bit 0 of parameter No.: 12 can be set whether the manual rapid traverse is enabled before the reference
position return.
4.1.3 Manual Feed & Manual Rapid Traverse Rate Selection
In the manual feed, select the manual feedrate by band switch, total 21 levels (0%--200%).
In the manual rapid traverse rate, 218MC, 218MC-H or 218MC-V can be selected override of the
285
VOLUME II
OPERATION
In the <MANUAL MODE>, press the feed axis
GSK218MC Series Machining Center CNC System Programming & Operation Manual
manual rapid traverse rate by
, and total 4 gears for the rapid
override: Fo, 25%, 50% and 100%. Fo speed is set by data parameter P93).
218MC-U1 can be modified by
and
buttons.
Note: The rapid override selection can be available for the following traverse rate.
(1) G00 rapid feed
(2) Rapid feed in canned cycle
(3) The rapid feed in G28
(4) Manual rapid feed
For example: When the rapid feedrate is 6 m/min, if the override is 50%, the speed is then 3 m/min.
4.1.4 Manual Intervention
VOLUME II
OPERATION
In the Auto, MDI and DNC modes, the program is converted to the manual mode during
operating after the feed holde is performed, and then the manual intervention should be operated.
After moving each axis, then convert at the previous operated method; when this program is operated
by
, each axis rapidly returns to the origin manual intervention point based upon the G00
mode, and then continue the operation program.
Detailed explanations:
1. If single block operation is switched on during the return operation, the tool will perform
the single dwell at the manual intervention point.
2. If the alarm or reset occurs in the manual intervention or return, this function will be
cancelled.
3. When using the manual intervention, it is important to carefully use the machine lock,
mirror and scaling function.
4. When the manual intervention is performed, it is note that the machining procedure and
machining shape to avoid damage the tool or machine tool.
The manual intervention operation is shown below:
286
Chapter Four Manual Operation
1. N1 block cutting workpiece
Tool
N2
Workpiece
N1
Block start
2. At the intermediate point A of the N1 block, the machine stops
after controlling the feed hold switch.
Tool
N2
Workpiece
A
N1
3. Move the tool to point B manually, and then operate
the machine tool again.
刀具
B
Manual
intervention
N1
N2
Workpiece
A
4. After the tool automatically returns to the point A based upon the
G00 speed, perform the remained section of the N1 program.
VOLUME II
OPERATION
B
Tool
N2
N1
A
Workpiece
Fig. 4-1-4-1
4.1.5 Workpiece Correction
In order to guarantee the machining accuracy (dimension, shape and position precision) of the
component and surface quality, it is necessary to correct the position of the workpiece or the fixture
for clamping the workpiece.
The common correction method contains: drawing, trial cut, etc. as for its character, GSK 218MC
CNC designs the correcting operation method for specially using the tool. For example, the center of
a rectangle workpiece X-Y plane is positioned based upon the trial cut halving correction method (It is
also called as Center Correction), the operation steps are shown below:
1) Start the spindle with a certain rotation speed.
2) System shifts to the display interface of the relative coordinate. Firstly correct the X direction:
Position to the one side of the workpiece along X axis based upon the operation of the
movement axis with manual mode; and then move downward to Z axis, so that the tool nose is
287
GSK218MC Series Machining Center CNC System Programming & Operation Manual
lower the workpiece surface; lastly, move toward the negative of the workpiece with the lower
speed (Usually, use the MPG feed mode), till the tool is just cut to stop of the workpiece. In this
case, press the
in the editing panel area, then the
, and the X coordinate sets
to zero. (If it sets to other values, you can use the same method, for example, input “X20” to
confirm by
.)
3) Similiarly, move the tool and cut one side along the negative direction, press
after
, and then complete the center operation. It is note that the
positioning, then the press
setting of the center does not change the absolute and machine tool coordinate values.
4) Move the tool to the axis which the relative coordinate displays as 0, that is, the center along
the X direction.
VOLUME II
OPERATION
5) In the “Setting” interface, select the “Workpiece coordinate” page, press the
then the
, and then the zero setting along X axis is executed.
6) The floating coordinate system can be set by G92 at the center of the XY (The XY value of the
relative coordinate is 0, the positioning point of the machine tool), as well, the XY machine
coordinate of this point records within the parameter of the G54～G59 coordinate coordinate
system for calling by system.
7) The operation is completed for correcting the rectangular workpiece center by using the trial
cutting center method.
Flexibly understand the method of the relative assignment and the center function setting to
improve the correction speed and enhance the convenient of operation.
Workpiece
Workpiece
X
X
Fig. 4-1-5-1
Note 1: This system is only input the coordinate at the relative position displayed. (The place where can be
modified the offset can also be set the position of the relative coordinate.)
288
Chapter Four Manual Operation
Note 2: It owns the operation function, which can be performed the addition and subtraction operations to the
displayed coordinate value, before the displayed coordinate is set.
Note 3: After the coordinate system is set, if the coordinate system set by G92 will lost due to the mechanical
zero return or coordinate systems G54～G59 calling; it may not lose if the mechanical coordinate records
to G54～G59 by parameter. The operator may flexibly set based upon their requirements; usually, it is
suggested to use the latter.
4.2 Spindle Control
4.2.1 Spindle Positive
Specify the S speed in MDI mode; press this button in the Manual/MPG/single-step mode,
spindle rotates CCW.
4.2.2 Spindle Negative
spindle rotates CW.
4.2.3 Spindle Stop
In the Manual/MPG/Single-step mode, spindle stops rotation by pressing this button.
4.2.4 Automatic Shift of Spindle
Select the spindle whether is the frequency control or I/O point control by bit 2 of parameter No. 1.
When NO:1#2=0, the spindle speed is controlled by S speed command to carry out the automatic
shift; at present, the system can be performed 3-shift control, and its corresponding top rotation
speed is set by parameter (P246, P247 or P248). When NO:1#2=1, the automatic shifting of the
spindle speed is controlled by I/O point; at present, the system can be both performed 3-shift control
(S1, S2 or S3) and modified the shifting addition output of the ladder diagram. The system may
automatically perform the corresponding shifting selection after executing the S speed command.
289
VOLUME II
OPERATION
Specify the S speed in MDI mode; press this button in the Manual/MPG/Single-step mode,
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Spindle motor speed
Max. speed
(10V)
The Max.
clamping
speed of the
spindle motor
The Min.
clamping
speed of the
spindle motor
Top rotation
speed of
gear 1
Top rotation Top rotation
speed of
speed of
gear 2
gear 3
Spindle
revolving
command (S
command)
Fig. 4-2-4-1
Note: The automatic shifting is enabled, detect the spindle shift and perform the S code by the shifting in-position
signal.
4.3 Other Manual Operations
VOLUME II
OPERATION
4.3.1 Coolant Control
:
The coolant can be shifted between the ON and OFF. The indicator ON means that the
power is turned on, OFF is turned off.
4.3.2 Lubrication Control
:
It is turned on by pressing the lubrication button; it is turned off by releasing it. The
indicator ON means that the power is turned on, OFF is turned off.
4.3.3 Chip-removal Control
:
The chip-revmoval can be shifted between the ON and OFF. The indicator ON means that
the power is turned on, OFF is turned off.
290
Chapter Four Manual Operation
4.3.4
Workping Indicator Control
:
The working indicator can be shifted between the ON and OFF. The indicator ON means
that the power is turned on, OFF is turned off.
VOLUME II
OPERATION
291
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
292
Chapter Five
CHAPTER FIVE
Single-Step Operation
SINGLE-STEP OPERATION
5.1 Single-step feed
Enter the signle-step mode by ,
machine tool moves based upon the step-length
defined by system each time in this mode.
5.1.1 Movement Amount Selection
Select a movement increment by any of the
, and the
, the single step
length (0.100) displays in the <POSITION> interface. (Refer to the Fig. 5-1-1-1)
Fig. 5-1-1-1
The machine tool corresponding axis moves 0.1mm by pressing the movement axis once.
218MC-U1 can be controlled by
buttons, and the modification and
debugging methods are identical with the above-mentioned.
293
VOLUME II
OPERATION
movement increment can be displayed on the page; for example, press the
GSK218MC Series Machining Center CNC System Programming & Operation Manual
5.1.2 Selection of Movement axis and Movement Direction
The feed axis and its direction buttons
or
, the X axis can be moved positively
or negative along the X axis direction button, press its corresponding button once, and the
corresponding axis moves the distance of the system single-step definition; the same as the Y and Z
axes. This system does not temporarily support the manual 3-axis movement at the same time, but
the 3-axis can be performed the zero return simultaneously.
5.1.3 Single-step Feed Explanations
The top clamping speed of the single-step feed is set by data parameter P155.
The single-step feedrate does not be controlled by the feedrate, rapid override.
5.2 Single-step Interruption
VOLUME II
OPERATION
When the program is operated in the Auto, MDI and DNC mode, shift the single-step mode to
perform the single-step interruption function after dwells. Single-step interrupition coordinate system
is same as the MPG one, and the operation function is also similar as the MPG (The electric MPG is
the Hand Pulse Generator---MPG, similarly hereinafter) one, refer to the Control of MPG Interruption
Operation in Section 6.2 of OPERTION.
5.3 Auxiliary Control in Single-step Operation
It is same as the manual operation mode, refer to the Section 4.2 and 4.3 in this manual.
294
Chapter Six MPG Operation
CHAPTER SIX
MPG OPERATION
6.1 MPG Feed
Enter the MPG mode by
, the machine tool movement can controlled by MPG in this
feed mode.
6.1.1 Selection of Movement Amount
Select a movement increment by any of the
, the MPG increment (0.100)
displays in the <POSITION> interface. (Refer to the Fig. 6-1-1-1)
Fig. 6-1-1-1
218MC-U1 can be controlled by
buttons, and the modification
and debugging methods are identical with the above-mentioned.
295
VOLUME II
OPERATION
increment can be displayed on the page; for example, press the
, and the movement
GSK218MC Series Machining Center CNC System Programming & Operation Manual
6.1.2 Selection of Movement Axis and Direction
In the MPG operation mode, select a axis to be controlled by MPG, press the corresponding
button, and then this axis can be moved by MPG.
In the MPG operation mode, if you want to move the X axis by MPG, press
, in this case,
the X axis can be moved by operating the MPG.
The feed direction is controlled by MPG rotation direction; refer to the manual made by machine
tool manufacturer. Generally, MPG CW is positive direction feed, and the CCW is the negative feed.
6.1.3 MPG Feed Explanations
1. The relationshisp between the MPG graduation and the Machine tool movement amount; refer to
the following table:
Table 6-1-3-1
VOLUME II
OPERATION
The movement amount of each garaduation on MPG
MPG increment (mm)
0.001
0.01
0.1
Machine tool movement value (mm)
0.001
0.01
0.1
MPG increment (inch)
0.001
0.01
0.1
Machine tool movement value (inch)
0.0001
0.001
0.01
2. The numerical values from the above-mentioned table are differ from the different mechanical
drivings; refer to the User Manual from the machine tool manufactory.
3. When the bit 0 of parameter No.: 56 sets to 1, the MPG movement value selects the absolute
operation. The speed for rotating the MPG can not more than the 5r/s, if does, the graduation and
movement value may inconsistent.
6.2 Control for MPG Interruption Operation
6.2.1 Operation of MPG Interruption
The operation during the MPG can be overlapped the automatic movement in the Auto operation
mode.
296
Chapter Six MPG Operation
Z
Cutter position in
Cutter position after the Auto mode
MPG interruption
Tool
Programming
cutting depth
Tool
The cutting depth
is the result of
MPG interruption
X
Fig. 6-2-1-1
The operations are shown below:
1) Shift to MPG mode after dwelling during the operation in the Auto mode.
2) Move the tool postion by MPG, for example, performing the up/down movement along Z
axis or the translation along X or Y axis, as wll the rotation along A axis can be reached to
the destination of the coordinate system modification.
3) Start it after shifting to the Auto mode, and workpiece coordinate holds invariable till to
coordinate recovers the actual value after the mechanical zero return is performed.
Note: Set whether using the MPG/Single-step interruption function by bit 3 of parameter No.: 56.
hold, and then perform the MPG interruption function, refer to the Fig. 6-2-1-2 for MPG interruption
coordinate system .
Fig. 6-2-1-2
The operation steps of MPG interruption coordinate system clear: Move the cursor to MPG
interruption coordinate system X flash by the X button, the coordinate system is cleared by
,
and the Y, Z axis shares with the same operation; When the zero return operation is performed, the
coordinate system is then automatically cleared.
297
VOLUME II
OPERATION
When a program is performed in the Auto, MDI or DNC mode, shift to the MPG mode after feed
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Note: When the alarm or resetting is generated during the coordinate system is adjusted by using the MPG
interruption function, the MPG interruption is then cancelled.
6.2.2 Relationships Between MPG Interruption and Other Fucntions
Table 6-2-2-1
Display
Relationship
Machine lock
MPT interruption movement machine tool is disabled after the
machine locking is enabled.
Absolute coordinate value
Absolute coordinate value does not change in MPG interruption
Relative coordinate value
Relative coordinate value does not change in MPG interruption
Machine tool coordinate value
The change value of the machine tool coordinate value is shifting
value caused by MPG rotation.
Note: The movement amount of MPG interruption is cleared when manual reference position return along each axis is
performed.
VOLUME II
OPERATION
6.3 Auxiliary Control During MPG Operation
Its operation method is absolutely same as the Manual, refer to the Section 4.2 and 4.3 in this
User Manual.
6.4 Electric MPG Drive Function
The component program operation can be controlled by rotating the MPG with hand, the
mechanism is operated along the tool path specified by machining program command, this function is
used for workpiece trial cutting and machining program detection.
Operation method:
The electric MPG drive function is enabled by setting the bit 1 of parameter No.: 59. In the Auto
mode, open the dry run, each axis of the system will not move after pressing the <CYCLE START>
button; in this case, the operation of the component operation can be controlled by rotating the MPG;
the faster the MPG rotation is, the faster the speed executed by program is; the slower the MPG
rotation is, the slower the speed executed by program is.
Note 1: The dry run is enabled after using the electric MPG drive function.
Note 2: In the single mode, the executiong of the single dwell is enabled.
298
Chapter Seven
Automatic Operation
CHAPTER SEVEN AUTOMATIC OPERATION
7.1 Selection of Auto Operation
1. Program loading in Auto mode
(a) Enter the Auto operation mode by
;
(b) Enter the【LIST】page display by
, find a destination program by moving the cursor;
(c) Confirm it by
.
2. Program loading in Edit Mode
(b) Enter the【LIST】page display by
(c) 按
;
, find a destination program by moving the cursor;
键进行确认。
(c) Confirm it by
.
(d) Enter the Auto operation mode by
;
7.2 Start of Auto Operation
After the desired program to be started is selected by the two methods in Section 7.1, the
program operates in Auto mode by pressing the
, and then observe the program operation
shifting to the <POSITION>, <MONITORING> or <FIGURE> interfaces, etc.
The program operation starts at the line where the cursor locates, and therefore, firstly check
299
VOLUME II
OPERATION
(a) Enter the editing operation mode by
GSK218MC Series Machining Center CNC System Programming & Operation Manual
whether the cursor is on the desired line before pressing the
, and confirm whether the modal
value is correct. If it starts from start line but the cursor does not locate at this line, press the
then the
,
to carry out the automatic operation program from start line.
Note: In the Auto mode, the workpiece coordinate system and basis offset value can not be modified during the
operation program.
7.3 Stop of Auto Operation
During the program Auto operation, the system provides 5 methods to stop the automatic
program:
1. Program sto (M00)
After the block with M00 is executed, program operation dwell, and the overall modal information
VOLUME II
OPERATION
is saved. The program continues after controlling the
.
2. Program selection stop (M01)
Before the program operation, if the
is pressed, the program dwells when it executes
the block containing the M01, and then the overall modal information is saved. The program
continues after controlling the
.
3. Press the
After pressing the
in the Auto operation mode, the machine tool shows the following
states:
1) Machine tool feed decelerates then stops;
2) When the dwell (G04 code) is performed, the timer stops then enters the feed hold state;
3) The rest of modal information is saved;
300
Chapter Seven
Automatic Operation
4) The program consecutively performs after pressing
.
4. Press the
Refer to the Section 2.3.1 OPERATION EXPLANATION VOLUME.
5. Press the ESP button
Refer to the Section 2.3.1 in this OPERATION EXPLANATION VOLUME.
In addition, when the program is operated in the Auto, DNC, MDI and MDI interface, the machine
tool can be stopped after shifting to other modes. Refer to the following items:
1) Shift to the Edit, MDI or DNC interface, the machine tool stops after performing the current
block.
2) Shift to the Manual, MPG or Single-step interface, the machine tool immediately stops after
the operation is interrupted.
3) Shift to the mechanical zero return interface, the machine tool decelerates then stops.
The system supports the automatic operation of any block from current machining program.
Refer to the following operation steps:
1. Enter the Manual mode by
, start the spindle and other miscellaneous function;
2. Operate each modal value of the program in the MDI mode, it is necessary to guarantee the modal
value is correct;
3. Enter the Edit operation mode by
; enter the program page display by
, and the
find the desired program to be machined in【LIST】.
4. Open the program, move the cursor before the block to be operated;
5. Enter the Auto operation mode by
6. Automatically operate the program by
;
.
Note 1: Confirm the current coordinate point is the previous block operation end positon (The current coordinate
point need not to be confirmed if the operated block is absolute programming and the G00/G01 movement) on
its operation block.
301
VOLUME II
OPERATION
7.4 Automatic Operation from Any Block
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Note 2: For example, if the this operated block is tool-change movement, firstly conform the current position
will not impact with the workpiece, etc.; to avoid the machine tool damage and personal injury.
7.5 Dry Run
The program can be inspected by “Dry run” before the program is machined; generally, it is used
matching with the “M.S.T Lock” or “Machine Lock”. Enter the Auto operation mode by
then press the
, and
(The indicator-ON on the button means the machine enters the dry run
state).
In the rapid feed, the program speed = dry run speed x rapid feedrate.
In the cutting feed, the program speed = dry run speed x cutting feedrate.
Note 1: Dry run speed is set by data parameter P86;
Note 2: Whether the dry run is enabled is set by bit 5 of parameter No.:12 during tapping.
Note 3: Whether the dry run is enabled is set by bit 6 of parameter No.:12 when the cutting feed is performed.
Note 4: Whether the dry run is enabled is set by bit 7 of parameter No.:12 in the rapid positioning.
VOLUME II
OPERATION
7.6 Single Block Operation
If you want to check the operation circumstance of the single bock, the “Program single block”
operation can be selected.
Press the
button (The indicator-ON on the button means that the single operation state
is already performed) in Auto, DNC or MDI mode. When the single block is operated, the system
stops operation after performing one block, and then continue performing the next block by
,
till the program operation is completed.
Note: During the G28, also, the single block can be stopped on the intermediate point.
7.7 Machine Locking Operation
Press the
button (The indicator-ON on the button means that the single operation state
is already performed) in the <AUTO> operation mode. In this case, each axis of machine tool does
302
Chapter Seven
Automatic Operation
not move, but the display of the position coordinate is identical with the machine movement, as well
the M, S or T can be performed; this function is used for program verification.
7.8 M.S.T Function Locking Operation
Press the
button (The indicator-ON on the button means that the single operation state
is already performed) in the <AUTO> operation mode. In this case, M, S or T code does not perform,
which is used for the program verification with the machine tool locking function together.
Note: M00, M01, M02, M30, M98 and M99 can be performed normally.
7.9 Feed, Rapid Trimming in Auto Operation
In the <AUTO>operation, the system can be changed the movement velocity by trimming feed or
rapid traverse rate.
in the Auto mode, its feed override can be
carried out 21-level real-time adjustment. Press
once, the feedrate increases one level,
each level is 10%, it will not increase any more till to 200%; the feedrate decrease one level by
once, each level is 10%; the bit 4 of parameter No.: 12 set whether the axis is stopped if the
override regards to Fo; if it sets to 0 without stopping, the actual rapid traverse rate is set by
parameter P93 (General-purpose for overall axes).
In the Auto mode, select the rapid traverse rate by
, the rapid
override can be carried out four-step adjustment: Fo, 25％, 50％ and 100％.
GSK218MC-H and GSK218MC-V CNC System can be selected the feedrate by its feed override
wave band switch
, and the feed override can be carried out 21-level real-time
adjustment.
GSK218MC-U1 is performed the feed override trimming by
and
, and
303
VOLUME II
OPERATION
Select the feedrate by
GSK218MC Series Machining Center CNC System Programming & Operation Manual
performed the rapid traverse override for trimming by
and
, its operations
are same as the above-mentioned.
Note 1: The value set by F in feed override trimming program
Actua feedrate = The value set by F x feed override
Note 2: The calculation of the rapid traverse speed value gained at the eventually trim by data parameter P88, P89
and P92 and the rapid override:
X axis actual rapid traverse speed = The value set by P88 x rapid override
The calculation method of the actual rapid traverse rate of Y and Z axes are shown as the above-mentioned.
7.10. Spindle Speed Trimming in Auto Mode
In the Auto mode, when the spindle speed controls by selecting the analog value, the spindle
then can be performed the trimming.
In the Auto mode, change the spindle speed by adjusting the spindle override based upon
VOLUME II
OPERATION
the ,
and the spindle override can be carried out 50％～120％ real-time
adjustments, total 8 levels.
The revolving override increases one level by pressing
once, each level is 10%, it will
not increase any more till to 120%.
The revolving override decreases one level by pressing
once, each level is 10%, the
spindle speed stops till to 50%.
GSK218MC-H/-V CNC System can be changed the spindle speed by adjusting the spindle
override by spindle override wave band switch
, and the spindle override can be carried
out the feed override can be carried out 50％～120％ real-time adjustments, total 8-level.
The actual speed of spindle = program command speed x spindle override. The top spindle
speed is determined by data parameter P258. It will be rotated based upon this speed if it exceeds
this numerical value.
304
Chapter Seven
7.11
Automatic Operation
Background Editing in Auto Mode
System supports the background editing function during the machining procedure.
In the Auto mode, enter the program display interface in <PROGRAM> during the program
operation, and then press the【PROGRAM】softkey, then enter the background editing interface; refer
to the Fig. 7-11-1:
VOLUME II
OPERATION
Fig. 7-11-1
Enter the program background editing interface by【B. EDITING】softkey, the editing of the
program is indentcial under the editing mode. Refer to the CHAPTER TEN PROGRAM EDITING
OPERATION of the OPERATION MANUAL; save and retreat from this interface by【B. EDITING】
editing program.
Note 1: It is suggest that the background editing file size is less than 3000 lines; otherwise, the machining
result may be affected.
Note 2: The background editing can be opened the foreground program, instead of editing or delecting the
foreground program.
Note 3: The background editing can not compile the operating foreground program.
305
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
306
Chapter Eight
MDI Operation
CHAPTER EIGHT MDI OPERATION
System can be both performed the MDI, parameter modification or offset, etc. and offered the
MDI operation function in the MDI mode, and it can be operated by directly inputting the code based
upon this function. The MDI data, parameter modification or offset, etc describes in the Interface
Display and Data Modification and Setting in CHAPTER THREE, as well, the MDI operation function
is also introduced in this chapter.
8.1 MDI Code Input
There are two input methods in MDI mode:
1. 【MDI】can be consecutively input multiple-block program;
2. 【CUR/MOD】can be input only one program.
In the【MDI】mode, the program input is same as the same editing mode, refer to the PROGRAM
EDITING OPERATION in CHAPTER TEN; The following will introduce the input in the【CUR/MOD】.
steps are shown below:
1) Enter the MDI operation mode by
2) Enter the program interface by
;
, then enter the【CUR/MOD】operation page by the
【CUR/MOD】softkey (refer to Fig. 8-1-1) :
3) After inputting the G00X50Y100 on keyboard in turn, confirm it by
; in this case, you
can view that the program is already input to the interface.
Refer to the following figure (Fig. 8-1-1 ):
307
VOLUME II
OPERATION
For example: Input a block G00 X50 Y100 from the【CUR/MOD】operation page, the operation
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 8-1-1
8.2 Operation and Stop of MDI Code Block
VOLUME II
OPERATION
After the code block is inputted based upon the Section 8.1, the MDI can be operated by
The code block operation can be stopped by
.
during the operation.
Note 1: The operation of MDI must be performed in MDI operation method!
Note 2: When the operation program in the MDI and CUR/MOD interface is performed in MDI mode, firstly treat
the inputted program in the CUR/MOD interface.
8.3 Modification and Clear of Filed Value in MDI Code Block
If the error occurs during the field input, cancel the input by
; if the error occurs after the
input is performed, input again the correct content to replace the error one or clear the overall
inputted contents by
, and then input again.
8.4 Conversion of Each Operation Mode
In the Auto, MDI or DNC mode, some programs are converted to MDI, DNC, Auto or Editing
308
Chapter Eight
MDI Operation
mode during the operation; the system stops the program after performing the current block.
In the Auto, MDI or DNC mode, the program converts to the single-step mode after dwells, the
single-stop function is then performed, refer to the single-step interruption in Section 5.2 of the
OPERATION MANUAL. Shift to MPG mode after dwells, and then the MPG interruption function is
performed, refer to the Manual Interruption in Section 6.2 of the OPERATION MANUAL. Shift to MPG
mode after dwells, and then the manual intervention function is performed, refer to the Manual
Intervention Function in Section 4.1.4 of the OPERATION MANUAL.
In the Auto, MDI or DNC mode, when the program is directly shifted to the single-step, MPG,
Manual, Zero-return mode during the operation, and the program is then stopped after decelerates.
VOLUME II
OPERATION
309
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
310
Chapter Nine
Zero Return Operation
CHAPTER NINE ZERO RETURN OPERATION
9.1 Concept of Machine Tool Zero (Mechanical Zero)
The machine tool coordinate system is the inherent one for a machine, its origin is called the
mechanical zero (or machine tool zero), also, it regards as Reference Point in this Manual which
described the mechanical origin by machine tool manufacturer; usually, it installs at the top traversal
along X, Y, Z, as the 4th and 5th axes positively. The mechanical zero point does not execute when the
CNC equipment is power on, it is better to perform the Auto or Manual mechanical zero return.
9.2 Operation Steps for Pulse Servo Mechanical Zero Return
, in this case, the “Mechanical
zero return” displays at the right corcer on LCD screen.
Fig. 9-2-1
2. Select the X, Y, Z, 4th or 5th axis to be returned the mechanical zero, the zero return direction is
determined by bit 0~4 of parameter No.7.
3. Machine moves along with the mechanical zero point. The machine moves (The movement
311
VOLUME II
OPERATION
1. Enter the mechanical zero return operation method by
GSK218MC Series Machining Center CNC System Programming & Operation Manual
speed is determined by data parameter P100～P104 P100～P104.) rapidly before the deceleration
point. The data parameters P342~P346 are set the zero return speed along each axis after touching
the deceleration switch. The speed of FL (It determines by data parameter P099) moves to
mechanical zero (that is, reference point) after departing from the stopper. The coordinate axis stops
to move and zero return indicator lights on after returning to the mechanical poont.
For example:
The 1st axis common incremental zero return is regarded as an example; the 1st axis begins to
impact the stopper with the higher speed F4000 (Data parameter P100 sets as 4000), and then pass
the stopper based upon the F500 (Data parameter P342 sets to 500) after touching the deceleration
switch, then slowly search the one-turn Z pulse signal of servo with F40 (Data parameter P99 sets to
40) after departing from the stopper, lastly, it immediately stops after gaining, refer to the Fig. 9-2-2.
Depart from the
stopper position
F4000
VOLUME II
OPERATION
Operate to the zero return stopper based
upon high speed
F500
Slow
One-turn signal
position
Stop position
F0
F40
Detect the
Z pulse
signal
Zero
return
stopper
tely
d ia
e
Imm stop
Stopper position
Fig. 9-2-2
9.3
Operation Steps for Mechanical Zero Return Specified by
Program
A G28 zero turn can be specified by program after bit 3 of parameter No.: 6 sets to 0, because
the detection of stroke stopper is shared the same effect with the manual mechanical zero turn.
9.4
Bus Servo Zero-Return Function Setting
There are three kinds of zero return methods when the system configures a bus servo, which are
separately common, high speed and multi-core absolute setting zero. We will separately introduce
the following setting methods.
312
Chapter Nine
Zero Return Operation
9.4.1 Common Zero Turn
Set the bit parameter No：0#0=1 and No：5#4=0, the system is performed the zero return based
upon the common one, which can be selected the zero return method such as the one-turn signal or
one-shot signal, and this zero return method can be used in the version of the system configuration
DA98B, GE2000 series increment method. Zero return along each axis is enabled in the zero return
mode.
The concrete operation steps are basically identical with the pulse servo zero turen; refer to the
Section 9.2 Operation Steps of Pulse Mechanical Zero Return.
9.4.2 High Speed Increment Zero Return
Set the bit parameter No：0#0=1 and No：5#4=0, the system is performed the zero return based
upon the high speed one, which can only be selected the one-turn signal zero return method, and this
method can be used in the version of the system configuration GE2000 series increment method.
Each axis zero valid in zero mode
single-core absolute, multi-core absolute version. The setting of parametr value of the data parameter
P347~P351 can be modified the single-core zero signal postion of the absolute encoder; Zero turn
along each axis is enabled in the zero return method.
Zero return steps:
1. Enter the mechanical zero return operation method by
, in this case, the
“Mechanical zero return” displays at the right corner of the LCD.
2. Select the X, Y, Z, 4th or 5th axis of the desired mechanical zero return, its direction of zero
return is set by bit parameters N0:7#0～N0:7#4.
3. Machine tool moves along with the mechanical zero direction at the rapid traverse rate (its
movement velocity is set by data parameter P100～P104) before the deceleration point; set the
zero return speed along each axis is set by data parameter P342~P346 after touching the
deceleration switch; Inquire the Z pulse one-turen signal position based upon the speed of the
data parameter P342~P346 after departing from the stopper, it decelerates and stops after
detecting, and then return to the mechanical zero (that is the reference point) based upon the
speed of the data parameter P354. The coordinate axis is stopped moving when returning to the
mechanical zero, and the zero indicator is turned on.
313
VOLUME II
OPERATION
Set the bit parameter No：20#7=0、No：20#6=1、No：20#5=0 to configure the GE2000 series
GSK218MC Series Machining Center CNC System Programming & Operation Manual
For example:
The 1st axis high-speed incremental zero return is regarded as an example; the 1st axis begins to
impact the stopper with the higher speed F4000 (Data parameter P100 sets as 4000), and then pass
the stopper based upon the F500 (Data parameter P342 sets to 500) after touching the deceleration
switch; search the one-turn Z pulse signal position of the servo based upon the F5000 speed after
departing from the stopper, it decelerates then stops after detecting, and then return to the
mechanical zero based on the F200 (The data parameter P354 sets to 200) speed, refer to the Fig.
9-4-2-1.
O ne-turn signal
position
Stop
F500~F0
position
D epart from the
stopper position
Stopper position
F4000
F500
F500
O perate to the zero return stopper w ith
high speed
Low
speed
D etect the Z
pulse signal
position
Zero
return
stopper
F200
De
ce
le r
at
e
to
s to
p
Z pulse signal
position feedback
VOLUME II
OPERATION
Fig. 9-4-2-1
9.4.3 Multi-Core Absolute Zero Setting
Set the bit parameters No：0#0=1, No：20#7=1, No：20#6=1 and No：20#5=1, configure the
GE2000 series multi-core absolute version, manually move each axis to the granted position of the
machine tool zero, then set the 1st axis zero position when bit parameter No：21#0=1, the 2nd axis
zero position when No：21#4=1, the 3rd axis zero position when No：21#2=1, the 4th axis zero position
when No：21#3=1 and the 5th axis zero position when No：21#4=1 in the MDI mode. In the zero return
mode, if the zero return indicator is turned on, the machine zero point setting is successful.
Note: It is hard to set the zero by this method, it is more convenient to set on the bus configuration interface.
This zero return mode can be directly set on the【
BUS CONFIGURATION】interface, refer to
the Display, Modification and Setting of Bus Servo Parameter in Section 3.3.5 for details.
For example:
The absolute encoder setting zero can be set the zero position based upon the absolute position
from the motor feedback. Set the bit parameter #20.7=1, #20.6=1, #20.5=1. Refer to the Fig. 9-4-3-1.
314
Chapter Nine
Zero Return Operation
Positive limit
Negative limit
Fig. 9-4-3-1 Absolute encoder zero setting
Note 1: Never attempt to operate the mechanical zero return, if your machine tool does not install the zero return
deceleration switch or set the mechanical zero.
Note 2: The indicator of corresponding axis is turned on when the mechanical zero return is ended.
Note 3: The zero return indicator is turned off when the corresponding axis does not at the mechanical zero point.
Note 4: Refer to the machine tool User Manual made by the manufacturer for the mechanical zero (reference point)
direction.
Note 5: Do not modify the zero return direction, feed axis direction and gear ratio dimension along each axis after the
mechnical zero is set,
Note 6: Refer to the Section 4.8 for CHAPTER FOUR INSTALLATION & CONNECTION in PLC & INSTALLATON
CONNECTION VOLUMN for the relevant parameter of mechanical zero return and all kinds of methods of mechanical
zero return.
VOLUME II
OPERATION
315
GSK218MC Series Machining Center CNC System Programming & Operation Manual
VOLUME II
OPERATION
316
Chapter Ten Edit Operation
CHAPTER TEN EDIT OPERATION
10.1 Edit of Program
The editing of the component program should be performed in the Edit operation mode. Enter
the editing operation method by
; enter the program interface by
then enter the editing and modification interface after pressing the【
on the panel;
PROGRAM】softkey (Refer to
the Fig. 10-1-1):
VOLUME II
OPERATION
Press【X】to enter the next page
Press【X】to enter the next page
Pres【W】to enter the next page
Fig. 10-1-1
Each operation, such as the replacement, cutting, copy, paste and restart, etc. can be performed
by pressing the corresponding softkey.
Before the program is compiled, the editing operation can only be performed by opening the
program switch. Refer to the Section 3.4.1 for details.
Note 1: The top lines of single program file are 100 thousand (lines).
Note 2: Refer to the Fig. 10-1-1, when the initial symbol “/” of the block is more than 1, the system still skips this
block even if the skip function does not start.
Note 3: The other methods can not be shifted during the correction is performed in the Auto mode; otherwise, the
unexpected circumstance may occur.
Perform the correction function in Auto mode, when the “/” symbol locates at the beginning of the block, the
317
GSK218MC Series Machining Center CNC System Programming & Operation Manual
program followed with the “/” will perform the correction function regardless of whether the skip function is
started or not.
10.1.1 Establishment of Program
10.1.1.1 Automatic Generation of Sequence Number
The “Automatic sequence number” sets to 1 based upon the Section 3.4.1 in OPERATION
(Refer to the Fig. 10-1-1-1-1).
VOLUME II
OPERATION
Fig. 10-1-1-1-1
In this case, the system will automatically insert a sequence number among blocks when the
program is edited, and the number incremental value of the sequence number can be set in the
series number incremental value.
10.1.1.2 Input of Program Content
1. Enter the Editing operation method by
2. Enter the program page display by
318
;
. (Refer to the Fig. 10-1-1-2-1):
Chapter Ten Edit Operation
Fig. 10-1-1-2-1
3. Input the number buttons
,
,
,
and
(For example,
,
display the O00002 followed with the data column, refer to the following Fig. 10-1-1-2-2:
Fig. 10-1-1-2-2
4. Establish a new program name by
, refer to the following Fig. 10-1-1-2-3:
319
VOLUME II
OPERATION
the establishment of the O00002 program name) in turn by the address button
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 10-1-1-2-3
5. Input the compiled program step by step, simultaneously, the program is automatically stored
after the complete to shift other working methods; if you want to shift other interfaces (such as
VOLUME II
OPERATION
the
), firstly press the
to save, and then complete the program input.
Note 1: In the Editing method, the system is temporarily not supported the single number.
Note 2: If you find the code word is incorrect when the program is input, cancel the input code by
.
Note 3: Up to 65 characters for the single input of the block.
10.1.1.3 Index of Sequence Number, Word and Line Number
Sequence number index is a sequence number within the index program. Generally, the
program can be performed or edited from the beginning of this sequence number. The skipped block
due to index does not affect to the CNC state. (The coordinate value, M, S, T code, G code, etc. of
the coordinate value in the skipped block does not affect to the coordinate value of CNC and the
modal value.)
If some one block from index program begins performing, in this case, the machine state, CNC
state should be checked. It can be operated when the corresponding M, S, T code and the setting of
the coordinate system, etc. are consistent.
The index of word, generally, uses the specified address word or numbers during the index for
the program editing.
The steps of sequence number, word and line number during the index program:
1. Selection method: <EDIT> or <AUTO> method.
2. Find the object program in【LIST】.
320
Chapter Ten Edit Operation
3. Enter to the object program by
.
4. Input the word or sequence number to be indexed, and find it by the
or
button.
5. If the line number in the program should be searched, you can input the desired line number
and then confirm it by
button.
Note 1: The index function is automatically cancelled when the sequence number or word indexes to the end of the
program.
Note 2: The sequence number, word and line number can be indexed in the【AUTO】and【EDIT】methods; however,
it can only be performed at the background editing interface in【AUTO】mode.
10.1.1.4 Positioning method of cursor
, display program screen.
a) Move the cursor one line upward by
, if the line of the cursor locates is more than
the end line of the previous one, the cursor then moves to the end of the last line.
b) Move the cursor one line downward by
, if the line of the cursor locates is more
than the end line of the next one, the cursor then moves to the end of the next line.
, if the cursor at the end line can be moved
c) Move the cursor one line rightward by
at the start of the next line.
d) Move the cursor one line rightward by
, if the cursor at the end start can be
moved at the end of the last line.
e) Scroll the screen upward by
f) Scroll the screen downward by
, cusor the moves to the last screen.
, cusor the moves to the next screen.
321
VOLUME II
OPERATION
Select the editing method, press the
GSK218MC Series Machining Center CNC System Programming & Operation Manual
g) Cursor moves to the beginning of its line by
.
h) Cursor returns to the start of the program by
＋
i) Cursor moves to the end line of its line by
.
.
j) Cursor moves to the end of the program by
＋
.
10.1.1.5 Insertion, Deletion and Modification of Word
Select the <EDIT>mode, press the
, and then display the program screen, lastly
position the cursor at the position to be edited.
VOLUME II
OPERATION
1. The insertion of a word
After the data is input, press the
, the system may insert the inputted content at the left
fo the cursor;
2. The deletion of a word
Position the cursor to the place to be deleted, press the
, the system may delete the
content where the cursor locates.
3. The modification of a word
Move the cursor to the place to be modified, and then input the modified content, then press the
, the system replaces the positioned content of the cursor inputted one.
10.1.1.6 Deletion of Single Block
Select the <EDIT> mode, press the
322
, and then enter the program screen, then move
Chapter Ten Edit Operation
the cursor to the initial line of the block to be deleted, lastly delete the cursor block by
＋
.
Note: The
can be input to delete (The cursor should be placed at the first line) the block regardless whether
the block is with or without the sequence number,
10.1.1.7 Deletion of Multi-Block
Delete to the block of the specified sequence number from the beginning of the current displayed
word.
N100 X100.0 M03 S2000; ..... N2233 S02 ; N 2300
M30 ;
Cursor current position
Delete this area
In the <EDIT> mode, enter the program display screen by
, position the cursor at the
object start position (Refer to the above-mentioned character N100) to be deleted; and the input the
last complete character in the multi-block to be cleared; for example, the S02 (Refer to the Fig.
10-1-1-7-1), and then press the
. The program between the cursor and address mark can
be deleted.
Note 1: Up to 100 thousand lines of the block deletion.
Note 2: If there are several same completed characters should be deleted in program, delete the program between
the completed character and cursor character with the search sequence downward.
Note 3: When multiple blocks are deleted with N+ sequence number, the N+ sequence number start position of
destination deletion should be located at the initial line of this block.
10.1.1.8 Deletion of Multiple Code Word
Delete to the specified code word from current displayed one.
323
VOLUME II
OPERATION
Fig. 10-1-1-7-1
GSK218MC Series Machining Center CNC System Programming & Operation Manual
N100 X100.0 M03 S2000; G01 X50.0 Y100.0 N2233 S02 ;
Cursor current position
Delete this area
Fig. 10-1-1-8-1
In the <EDIT> mode, enter the program display screen by
, position the cursor at the
object start position (Refer to the above-mentioned character N100) to be deleted; and the input the
last complete character in the multi-block to be cleared; for example, the Y100.0 (Refer to the Fig.
10-1-1-8-1), and then press the
. The program between the cursor and address mark can
be deleted.
Note 1: If the N+ sequence number lies among the blocks, the system regards that it is the code word treatement.
10.1.2 Deletion of Single Block
VOLUME II
OPERATION
When some one program in the memory should be deleted, refer to the following steps:
a) Select <EDIT>operation method;
b) Enter the program display page, there are two methods to delete the program:
1. Input the address
,
or
; input the program name (input the numerical button
,
, in this case, the O0002 program is regarded as an example);
the program in the memory is deleted by
.
2. Select the【LIST】interface in program interface, select the program name to be deleted by
cursor, the system state column prompts “Confirm deleting the current file?” by
the state column shows “Deletion Successful” by
, and then
again, lastly, the selected program by
cursor can be deleted.
Note 1: If only one program file is performed, under the editing mode program (list) interface, the program name will
become O00001 and the program content is deleted regardless of the program name is O00001 or not; when the
multiple program files are performed, the program content and name of O00001 will be deleted together.
324
Chapter Ten Edit Operation
10.1.3 Deletion of Overall Programs
The overall programs in the memory should be deleted, refer to the following steps:
a) Select the <EDIT>operation mode;
b) Enter the program display screen;
c) Input the address
;
d) Input the address
,
,
,
,
e) The overall programs in the memory are deleted by
and
in turn;
.
10.1.4 Program Copy
The current program copies and saves as a new program name:
b) Enter the program display page; selet the desired program to be copied by cursor in【LIST】
interface, enter the program display interface by
c) Press address button
;
, and then input a new program name;
d) The file is copied by【COPY】software, and then enter a new program editing interface.
e) A copied new program name can be viewed by returning to the【LIST】.
The copy of the program can also be performed at the program editing page (Refer to the Fig.
10-1-1):
1. Press the address button
, and then input a new program number;
2. The file is copied by【COPY】softkey, and then enter the new program editing interface.
3. A copied new program name can be viewed by returning to the【LIST】.
10.1.5
Copy and Paste of Block
The operation steps for the copy and paste of blocks are shown below:
a) Cursor moves to the start of the block to be copied.
325
VOLUME II
OPERATION
a) Select the <EDIT>mode
GSK218MC Series Machining Center CNC System Programming & Operation Manual
b) Input the last character of the block to be copied.
c) Press
+
buttons, the program between the cursor and character input are
copied.
d) Move the cursor to the position to be pasted, press the
+
buttons or
【PASTE】softkey, the paste is then completed.
The copy and paste of the block also can be performed in the program editing page (Refer to the
Fig. 10-1-1):
1. Cusor moves to the start of the block to be copied.
2. Input the last character of the block to be copied.
3. Press the【COPY】softkey, the program copy is completed between the cursor and character
input.
4. Cursor moves to the desired paste position, the paste is then completed by【PASTE】softkey.
Note 1: If there are several same completed characters should be copied in program, copy the program between the
completed character and cursor character with the search sequence downward.
VOLUME II
OPERATION
Note 2: If the copy method is performed by N+ sequence number in program, the program of line is copied between
the cursor start and N+ sequence number. The N+ sequence number should be located at the beginning of the
block, the copy is unsuccessful in other places.
Note 3: Up to 100 thousand lines of the block copy.
10.1.6 Cut and Paste of Block
The operation steps of block cut:
a) Enter the program editing page (Refer to Fig. 10-1-1).
b) Cusor moves to the start of the block to be cut.
c) Input the last character of the block to be cut.
d) Press【CUT】softkey, program is cut to the paste
e) Cursor moves to the position to be pasted, the paste is then completed by pressing the
【PASTE】softkey.
Note 1: If there are several same completed characters should be cut in program, cut the program between the
completed character and cursor character with the search sequence downward.
Note 2: If the cut method is performed by N+ sequence number in program, the program of line is cut between the
cursor start and N+ sequence number.
Note 3: When the program name shares a same block with the program content in the editing method program
interface, the character followed with the program name can be performed the copy operation for the system
instead of cutting operation.
326
Chapter Ten Edit Operation
10.1.7 Replacement of Block
The operation steps of block replacement:
a) Enter the program editing page (Refer to the Fig. 10-1-1).
b) Cursor moves to the character to be replaced.
c) Input the replaced content.
d) Press the【REPLACEMENT】softkey, the system replaces the content positioned by cursor
and the overall same contents in block as the one from input.
Note: This operation is only performed for character instead of executing the integrated block.
10.1.8 Rename of Program
The current program name changes into another name:
a) Select <EDIT>operation method;
b) Enter the program display interface (Cursor specifies the program name);
d) Press
VOLUME II
OPERATION
c) Input the address
, and then input a new program name;
, the file name is then completed.
10.1.9 Program Restart
This function is used for the program operations when the accident of the automatical motion
generates, such as the tool broren, power-off, ESP, rest, etc. The system returns to the program
breakpoint and performs continuely based upon the reatart function after the accident is eliminated.
The operation steps of the program restart:
1. Resolve the machine tool accident. For example, tool-change, offset alternation and
mechincial zero turen, etc.
2. In the <AUTO>mode, press the
3. Enter the program interface by the
button on the panel.
on the operation panel, and then enter the
sub-menu by the【PROGRAM】software below the LCD screen, page to the last one of the
327
GSK218MC Series Machining Center CNC System Programming & Operation Manual
sub-menu by pressing 【 X 】 twice, enter the program restart interface by pressing the
【RESTART】. Record the different codes between the current modal and preload one.
(Refer to the Fig. 10-1-9-1).
Fig. 10-1-9-1
VOLUME II
OPERATION
4. Shift to <MDI>mode, enter the CUR/MOD interface by pressing the【CUR/MOD】softkey, input
the corresponding modal code and M code based upon the preload modal value in the Fig.
10-1-9-1.
5. In the mode of returning the <AUTO>, press the
on the panel, and then press the
, the program moves to the start (That is, the intervention point of the previous
block) of the interruption block according to the sequence before the coordinates (1) (2)
and (3) based upon the dry run speed, and the machining is restarted again.
Explanations:
1. The (1) (2) and (3) before the coordinate syste is movement sequence of which each axis
moves to the restart position of the program, and its sequence is determined by data parameter
P376.
2. The single block is switched on when the coordinate system restarts the position movement,
the tool may stops after completing a axis direction movement. The intervention can not be
performed by shifting to the MDI mode during the execution.
3. The movement method along Z axis can be controlled by bit 0 of parameter No.: 49. (0：G00,
1：G01)
Note 1: The operation can be performed at an arbitary position, therefore, detect whether the tool will impact with the
328
Chapter Ten Edit Operation
workpiece or other object when moving to the program restart position, if does, the program restart can only be
performed after the tool moves to the places without any abstruction.
Note 2: The block of the program restart maybe not be interrupted in the halfway, the operation can be be restarted
from any block; its method is identical with the above-mentioned. It is only different that the N line number of the
preload modal value is directly defined by the direction button “↓” in the “MDI” mode at the 4th step, and then
confirm it by “INPUT” button. You can input the corresponding modal code and M code after entering the
CUR/MOD interface again.
Note 3: Never attempt to perform the restart when the restart block indexes to the execution period of program restart;
otherwise, the program start should be performed again at the 1st step.
Note 4: The reference position return should be performed before performing the restart after the power is turned on, if
the machine tool does not install the absolute position detector (absolute encoder).
Note 5: The program restart function does not support the form with the sub-program;
Note 6: The program restart function does not support the programs with the rotation, mirror image, scaling or polar
coordinate modal.
Note 7: The program restart function does not support the canned cycles programs;
Note 8: The program restart function does not support the DNC on-line machining program.
Note 9: The program restart function does not support macro programs (Including Type A, B).
10.2
VOLUME II
OPERATION
10.2.1
Program Administration
Index of Program List
Press the
buttin entering the program list display interface by controlling the【LIST】
softkey in the program interface (Refer to the Fig. 10-2-1-1):
Memory
information
Program quantity
information
Program list
Program
preview
Fig. 10-2-1-1
1) Open the program
Open a specified program: O + series number + input (or EOB) or series number + input (or
329
GSK218MC Series Machining Center CNC System Programming & Operation Manual
EOB)
A new program will be established if the input series number is null in the editing mode.
2) Delete the program:
1. Editing method
Delete the specified program by DEL.
2. Edit mode O + series number + DEL or Series number + DEL.
10.2.2 Quatity of Storage Program
Up to 400 can be stored at the system program, the sotred quantity can be view the Section
10.2.1 for the Program Number Information on the Program List Display Interface.
10.2.3 Storage Capacity
Refer to the Program Number Information on the Program List Display Interface in Section
10.2.1 for the concrete storage capacity.
VOLUME II
OPERATION
10.2.4 Check of Program List
Up to 6 CNC program names can be displayed at the program list display page once, if it is more
than 6, the display can not be performed within a page; in this case, you can use the page button to
display it. In succession, the LCD will display the CNC program name at the next page. LCD will
repeatedly show the overall CNC program names if you control the page button again and again.
10.2.5
Locking of Program
This system sets a program switch to avoid that the user program is being modified or deleted by
others. After the program is edited, the program can be locked by closing its switch, and the user can
not perform the program compilation any more, refer to the Section 3.4.1 for details.
330
CHAPTER ELEVEN
SYSTEM COMMUNICATION
The system can be communicated with the PC terminal or U disk by its interface to carry out the
data transmission or DNC on-line machining.
11.1 Serial Port Communication
Serial port communication preparation work:
1. The computer port (COM port) is connected with the RS232 of the system by serial cable.
2. Open the PC terminal GSK Com serial port communication software.
Note: GSK Com serial port communication software is Windows interface, which is suitable for the Win98,
WinMe, WinXP and Win2000.
3. The setting of the GSK Com serial port communication software:
(1) Select the available GSK218M (The transmission data error may occur if other system
types are selected);
(2) Click the “Series port” menu, set the Baud rate in the “Series Setting” dialog frame, and
the Baud rate selects 115200 (It is corresponding with the default value of the data parameter P002)
when the data is transmitted; the Baud rate selects 38400 (It is corresponding with the default value
of the data parameter P001) when DNC is on-line machining.
Program Start
Directly operate the Comm218M.exe program. The interface is shown below after the program is
started.
331
APPEDIX
11.1.1
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 11-1-1-1
11.1.2
Function Introduction
APPEDIX
1. File menu
The file menu contains some functions, such as the New, Open and Save the program file,
Print and Print setting, the file list for current opening file, etc.
2. Edit menu
Edit menu contains of cut, copy, paste, retraction, reach, replacement etc.
3. Series port menu
It is used for opening and setting of the series port.
4. Transmission method menu
It contains of the DNC transmission method, file delivery transmission method, file
reception transmission method.
5. Menu check
The display and hiding of tool and state bars.
6. Help menu
The software information for this software.
332
11.1.3
Series Port Data Transmission
The operation steps are shown below:
1) Select <MDI>operation mode;
2) Enter the setting page by
, set the I/O channel as 0 or 1.
3) Enter the setting (password) page by【PASSWORD】softkey, input the corresponding level
authority password. Refer to the Setting and Modification of Password Authority in Section
3.4.5.
4) Enter the setting (data treatment) page by
position by
or
, move the cursor to the detstination
.
A. Data output (CNC→PC)
1. System prompts “Waiting for the transmitting….” by pressing the【DATA OUTPUT】softkey.
2. Click
button (Alternatively, select the “Accept the file” in the
“Transmission mode” draw-down menu on the GSK Com series port communication
software, and then the “Accept the file” dialog frame is shown, refer to the Fig. 11-1-3-1.
APPEDIX
Fig. 11-1-3-1
333
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3. Click the
button in acceptance file dialog frame, and then gain the file list at
the CNC port, refer to the Fig. 11-1-3-2.
Fig. 11-1-3-2
4. Select the desired file to be accepted (Multiple files can be accepted), and then press the
button, the file begins to acceptance, refer to the Fig. 11-1-3-3.
APPEDIX
Fig. 11-1-3-3
5. After the file is performed the acceptance, the dialog state bar shows “Accepted”. Refer to
the Fig. 11-1-3-4.
Fig. 11-1-3-4
334
B. Data input (PC→CNC)
1. System prompts “Waiting for the transmitting….” by pressing the【DATA INPUT】softkey.
2. Click
button (Alternatively, select the “Deliver the file” in the
“Transmission mode” draw-down menu on the GSK Com series port communication software,
and then the “Deliver the file” dialog frame is shown, refer to the Fig. 11-1-3-5.
Fig. 11-1-3-5
3. Click the
button in acceptance file dialog frame, and then the selection
dialog frame shows, refer to the Fig.11-1-3-6.
APPEDIX
Fig. 11-1-3-6
4. In the selection dialog:
The user sub-area should be selected when the CNC component program and user program
are delivered; the system sub-area should be selected when the files suchas the ladder diagram
(PLC), parameter (PLC), system parameter value, tool compensation value, pitch compensation
value and system macro variable, etc. are transmitted.
5. Select the desired file to be accepted (Multiple files can be delivered), after the sub-area is
selected, and then click the
button, the file delivers, refer to the Fig. 11-1-3-7.
335
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 11-1-3-7
6. The dialog frame state displays “Delivered” after the file is performed the delivery. Refer to
the Fig. 11-1-3-8.
APPEDIX
Fig. 11-1-3-8
Note 1: It is necessary to ensure the Baud rate setting is correct before the data transmission, the series port cable
connection is reliable.
Note 2: Never attempt to perform the system shifting or page oerate; otherwise, the serious error may occur.
Note 3: LADCHI**.TXT file is disabled after introducing to system, it can be enabled after the power is turned off.
11.1.4
Series Port DNC ON-Line Machining
Operation steps:
1. CNC port setting:
1) Enter to the setting page by
, set the I/O channel to 0 or 1.
2) Select the <DNC>operation method; in this case, the system prompts “DNC is already
performed,
336
2. The setting of series port communication software
1) Click the “series port” menu, and then set the baud rate in the “Series port setting” dialog
frame, the Baud rate set to 38400.
2) When the system I/O channel sets to 0, the “DNC agreement” in the “Transmission
method” drop-down menu should be selected the Xon/Xoff;
When the system I/O channel sets to 1, the “DNC agreement” in the “Transmission
method” drop-down menu should be selected the XModem;
3. Open the CNC program file. The program file can be opened by the “Open” button on the file
menu or the
button on tool bar, refer to the Fig. 11-1-4-1 (Further edit the program
file to the series port communication software).
APPEDIX
Fig. 11-1-4-1
4. DNC transmission. The data delivers by clicking the
on tool bar or the “DNC
transmission” on the “Transmission mode” drop-down menu. When the system I/O channel
sets to 0, PC directly delivers with PC common-use method; in this case, the DNC
transmission dialog frame displays the state of file transmission, which includes the delivered
file name, delivered byte, line number, and the transmission time and speed (type/second),
refer to the Fig. 11-1-4-2. When the system I/O channel sets to 1, PC delivers based upon the
data packet; in this case, the dialog frame displays the state of file transmission, which
337
GSK218MC Series Machining Center CNC System Programming & Operation Manual
contains the delivered data packet and the times of the retransmission; refer to the Fig.
11-1-4-3:
Fig. 11-1-4-2 The system I/O channel sets to 0
Fig. 11-1-4-3 The system I/O channel sets to 1
APPEDIX
Note: 1. The series port communication software can not be performed other operations other than the end
transmission during the DNC transmission.
2. M99 regards as M30 in DNC mode.
3. Cancel the operation by
after the machining is completed.
11.2 USB Communication
11.2.1
Brief & Precaution
Precautions:
1. Set the I/O channel to 2 in <SETTING> interface.
2. The suffix name of CNC program should be .txt、.nc or .CNC, and stored at the U disk root directory;
otherwise, the system will not be read.
3. Never attempt to pull out the U disk when transmitting the communication by USB, to avoid the
338
product fault or unexpected result.
4. The U disk can be pulled out when the indicator of U disk does not flash after the U disk
communication operation is completed, to guarantee that the data transmission is executed.
11.2.2 USB Component Program Operation Steps
In the <MDI MODE>, move the cursor to “CNC component program” by direction button
or
after entering the setting (data treatment) interface. Enter the following operation
interface by softkey【DATA OUTPUT】or【DATA INPUT】, refer to the Fig. 11-2-2-1:
APPEDIX
Fig. 11-2-2-1
1. Copy the CNC program file from system disk to U:
a. Shift the cursor to the file list table by direction button
b. Move the cursor by
or
.
, select the CNC program file in system disk to be
copied.
c. The system prompts “Copy to U disk? New file name” by【COPY】softkey; refer to the
following figure (Fig. 11-2-2-2)
339
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Fig. 11-2-2-2
d. If the CNC program file does not need to be renamed, it can be directly copied by <INPUT>
button.
If the CNC program file should be renamed, input the new program number (For example, O10,
O100) by <CANCEL>, and the CNC program file then can be copied by <INPUT> again.
If the U disk stores at the program file with a same name, the system may prompt “RENAME
AGAIN”, therefore, it is necessary to input the new program numbers (for example: O10, O100); and
then the CNC program file can be copied by <INPUT> button.
2. Copy the CNC program file to system disk from U disk:
APPEDIX
a. Shift to the display interface of the U disk file list by【U DISK】softkey.
b. Shift the cursor to the file list table by direction button
c. Move the cursor by
or
.
, select the CNC program file in U disk to be copied.
The system prompts “Copy to system disk? New file name” by【COPY】softkey; refer to the
following figure (Fig. 11-2-2-3)
340
Fig. 11-2-2-3
d. If the CNC program file does not need to be renamed, it can be directly copied by <INPUT>
button.
If the CNC program file should be renamed, input the new program number (For example, O10,
O100) by <CANCEL>, and the CNC program file then can be copied by <INPUT> again.
If the system disk stores at the program file with a same name, the system may prompt
“RENAME AGAIN”, therefore, it is necessary to input the new program numbers (for example: O10,
O100); and then the CNC program file can be copied by <INPUT> button.
off.
3. Delete a file from system disk/U disk:
a. Move the cursor by
or
, select the CNC program file in the system disk/U
disk to be deleted.
b. “Confirm deleting the current file?” prompts at the botoom of the interface by【DELET】softkey;
cancle the file deletion by <CANCEL>; the file is deleted by <INPUT>button.
11.2.3 USB DNC Machine Operation Steps
1. In the <Setting> interface, set the I/O channel to 2. Refer to the Section 3.4.1 in OPERATION for
details.
2. Insert the U disk.
3. The system shifts to DNC mode by <DNC>button, in this case, prompt shows at the bottom of
the screen: “Select the machining file in USB list”; enter the program interface by <PROGRAM>,
341
APPEDIX
Note: The LADCHI**.TXT file is disabled after transferring to the system, it can be enabled after the power is turned
GSK218MC Series Machining Center CNC System Programming & Operation Manual
and then【LIST】, the USB program list table shows; select the program to be machined by moving
the cursor, open this program by <INPUT>, then press the <CYCLE START>, and then perform the
DNC machining.
Note: In the USB program list page, when the character numbers of program name is less than or equals to 6, the
start of program can be previewed; when the character numbers of program name is more than 6, the start of
program can not be previewed. When the character numbers of program name is more than or equals to 8, the
system is only displayed as abbreviation and can not be previewed the start of program.
11.2.4 Retreat from U Disk Operation Interface
1. Pull out the U disk when the indicator of the U disk does not flash.
Retreat from【SETTING (DATA TREATMENT)】interface by【RETURN】softkey.
APPEDIX
342
APPENDIX
APPEDIX
343
GSK218MC Series Machining Center CNC System Programming & Operation Manual
APPEDIX
344
Appendix One GSK218MC Parameter List
APPENDIX ONE
GSK218MC SERIES PARAMETER LIST
Parameter Explanation
The parameter can be dividied into the following types based upon the types of the data:
Two data types and its enabled range of the data value
Data
Enabled data
type
range
Bit-type
0 or 1
It determines
Data-type
based upon the
data range.
Remark
The default value provided by system can be modified its
setting based upon the user’s requirements.
The default range and value provided by system can be
modidified its setting based upon the user’s requirements.
1. Each data consists of 8-digit for the bit parameter, and each bit owns different meanings.
2. In the above-mentioned table, generally, the data value range of each data type is the enabled
range. Actually, the concrete parameter value range is different. Refer to the detailed
explanations for each parameter.
[Example]
APPEDIX
(1) The meaning of bit parameter
Data No.
BIT7
BIT6
BIT5
BIT4
BIT3
BIT2
BIT1
BIT0
(2) The meaning of data parameter
0 2 1
Data No.
Data
Note 1: The null position in parameter explanation and the parameter number on the screen but
without recording in the parameter table are backup for the extend in the future, so it is
necessary to set as 0.
Note 2: The 0 or 1 in the parameter does not specify the concrete meaning; 1: YES; 0: NO.
Note 3: INI sets to 0; parameter that sets the unit linear axis is mm, mm/min when the metric input is performed; the
basis unit of the rotation axis is deg, deg/min.
INI sets to 1; parameter that sets the unit linear axis is inch, inch/min when the inch input is performed; the basis
unit of the rotation axis is deg, deg/min.
345
GSK218MC Series Machining Center CNC System Programming & Operation Manual
1. Bit Parameter
System parameter No.
0 0 0
PBUS
MODE
SVCD
SEQ
MSP
CPB
INI
INM
PBUS
=1: The transmission method of the drive is bus type.
=0: The transmission method of the drive is pulse type.
INM
=1: The least movement unit of the linear axis is inch method
=0: The least movement unit of the linear axis is metric method
INM sets to 0, and when the metric input executes: the basis unit of the linear axis is mm,
mm/min; the basis unit of rotation axis is deg, deg/min.
INM sets to 1, and when the inch input executes: the basis unit of the linear axis is inch,
inch/min; the basis unit of rotation axis is deg, deg/min.
INI
=1: Inch input
=0: Metric input
INM sets to 0, and when the metric input executes: the basis unit of the linear axis is mm,
mm/min; the basis unit of rotation axis is deg, deg/min.
INM sets to 1, and when the inch input executes: the basis unit of the linear axis is inch,
inch/min; the basis unit of rotation axis is deg, deg/min.
CPB
=1: Pulse and Ethernet are simultaneously used.
=0: Pulse and Ethernet are not simultaneously used.
MSP
=1: Use the dual-spindle control.
APPEDIX
=0: Do not use the dual-spindle control.
SEQ
=1: Automatically insert the sequence number.
=0: Do not automatically insert the sequence number.
SVCD
=1: Use the bus servo card.
=0: Do not use the bus servo card.
MODE
=1: High-speed & high-accuracy mode, it can not be modify the #15.0 and
#17.0 but supporting the 4-axis 3-linkage.
=0: Common mode, when the high-speed & high-accuracy mode sets to the
common one, #15.0 sets to 1 by default.
Standard setting: 1 0 0 0 0 0 0 1
System parameter number
0 0 1
RASA
RAS5
RAS4
RAS3
RAS2
=1: Use the absolute grating scale.
=0: Do not use the absolute grating scale.
SBUS
346
=1: Spindle drive is bus control method.
RAS1
SPT
SBUS
RASA
Appendix One GSK218MC Parameter List
=0: Spindle drive is non-bus control method.
SPT
=1: I/O point control.
=0: Frequency-conversion or others
RAS1
=1: Use the grating scale by setting the 1st axis.
=0: Do not use the grating scale by setting the 1st axis.
RAS2
=1: Use the grating scale by setting the 2nd axis.
=0: Do not use the grating scale by setting the 2nd axis.
RAS3
=1: Use the grating scale by setting the 3rd axis.
=0: Do not use the grating scale by setting the 3rd axis.
RAS4
=1: Use the grating scale by setting the 4th axis.
=0: Use the grating scale by setting the 4th axis.
RAS5
=1: Use the grating scale by setting the 5th axis.
=0: Do not use the grating scale by setting the 5th axis.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0 0 2
DEC1
DEC5
DEC4
DEC3
DEC2
DEC1
=1: Deleration is performed when the deceleration signal is 1 and the 1st axis
reference position returns.
=0: Deleration is performed when the deceleration signal is 0 and the 1st axis
reference position returns.
APPEDIX
DEC2
=1: Deleration is performed when the deceleration signal is 1 and the 2nd axis
reference position returns.
=0: Deleration is performed when the deceleration signal is 0 and the 2nd axis
reference position returns.
DEC3
=1: Deleration is performed when the deceleration signal is 1 and the 3rd axis
reference position returns.
=0: Deleration is performed when the deceleration signal is 0 and the 3rd axis
reference position returns.
DEC4
=1: Deleration is performed when the deceleration signal is 1 and the 4th axis
reference position returns.
=0: Deleration is performed when the deceleration signal is 0 and the 4th axis
reference position returns.
=1: 第5轴参考点返回时减速信号为1时减速
DEC5
=1: Deleration is performed when the deceleration signal is 1 and the 5th axis
reference position returns.
=0: Deleration is performed when the deceleration signal is 0 and the 5th axis
reference position returns.
Standard setting：0 0 0 0 0 0 0 0
347
GSK218MC Series Machining Center CNC System Programming & Operation Manual
System parameter number
0
0
3
DIR5
DIR4
DIR3
DIR2
DIR1
=1: The 1st axis feed direction is reverse.
DIR1
=0: The 1st axis feed direction is positive.
=1: The 2nd axis feed direction is reverse.
DIR2
=0: The 2nd axis feed direction is positive.
=1: The 3rd axis feed direction is reverse.
DIR3
=0: The 3rd axis feed direction is positive.
=1: The 4th axis feed direction is reverse.
DIR4
=0: The 4th axis feed direction is positive.
=1: The 5th axis feed direction is reverse.
DIR5
=0: The 5th axis feed direction is positive.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
0
4
SK0
STME
TMES
=1: Tool-setter is already installed.
TMES
=0: Tool-setter does not install.
=1: Tool length measurement value can be written into the reference offset.
STME
=0: Tool length measurement value can not be written into the reference offset.
=1: SKIP is regarded as signal input when it is set to 0.
APPEDIX
SK0
=0: SKIP is regarded as signal input when it is set to 1.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
0
5
DOUS
HSRZ
ISC
=1: The least movement unit 0.0001mm&deg,0.00001inch.
ISC
=0: The least movement unit 0.001mm&deg,0.0001inch.
=1: High-speed zero return is enabled.
HSRZ
=0: High-speed zero return is disabled.
=1: Dual-drive tool uses the grating position.
DOUS
=0: Dual-drive tool does not use the grating position.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
348
0
6
MAOB
ZPLS
SIOD
SJZ
AZR
JAX
ZMOD
ZRN
Appendix One GSK218MC Parameter List
=1: Reference point does not establish, specify the code other than G28 in
ZRN
Auto operation, system alarms.
=0: Reference point does not establish, specify the code other than G28 in
Auto operation, system does not alarm.
=1: Zero return mode selection: Before the block.
ZMOD
=0: Zero return mode selection: After the block.
=1: The control axis at the same time of the manual reference point return:
JAX
single axis.
=0: The control axis at the same time of the manual reference point return:
multiplication axes.
=1: The G28 command when the reference point does not establish: Alarm
AZR
=0: The G28 command when the reference point does not establish: Use the
block
=1: Reference point memories.
SJZ
=0: Reference point does not memory.
=1: Mechanical zero return deceleration signal performs via PLC logic
SIOD
calculation.
=0 Mechanical zero return deceleration signal directly reads.
=1: Zero return method selection: with one-turn signal.
ZPLS
=0: Zero return method selection: without one-turn signal.
=1: Zero return method selection without one-turn signal: B method.
MAOB
=0: Zero return method selection without one-turn signal: A method.
APPEDIX
Standard setting：1 1 1 0 0 0 0 1
System parameter number
0
0
ZMI1
7
ZMI5
ZMI4
ZMI3
ZMI2
ZMI1
=1: Set the 1st axis reference point return direction: =0: Set the 1st axis reference point return direction: +
ZMI2
=1: Set the 2nd axis reference point return direction: =0: Set the 2nd axis reference point return direction: +
ZMI3
=1: Set the 3rd axis reference point return direction: =0: Set the 3rd axis reference point return direction: +
ZMI4
=1: Set the 4th axis reference point return direction: =0: Set the 4th axis reference point return direction: +
ZMI5
=1: Set the 5th axis reference point return direction: =01: Set the 5th axis reference point return direction: +
Standard setting：0 0 0 0 0 0 0 0
System parameter number
349
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0
0
8
AXS5
AXS4
AXS3
AXS2
AXS1
A4TP
RAB
=1: The 1st axis sets to rotation axis.
AXS1
=0: The 1st axis sets to linear axis.
=1: The 2nd axis sets to rotation axis.
AXS2
=0: The 2nd axis sets to linear axis.
=1: The 3rd axis sets to rotation axis.
AXS3
=0: The 3rd axis sets to linear axis.
=1: The 4th axis sets to rotation axis.
AXS4
=0: The 4th axis sets to linear axis.
=1: The 5th axis sets to rotation axis.
AXS5
=0: The 5th axis sets to linear axis.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
0
9
PD5
PD4
PD3
PD2
PD1
=1: Each axis rotates nearest when it regards as the rotation axis.
RAB
=0: Each axis does not rotates nearest when it regards as the rotation axis.
=1: 4-axis linkage system.
A4TP
=0: Non-4-axis linkage system.
=1: The 1st axis pulse direction of the Non-bus servo is negative.
PD1
APPEDIX
=0: The 1st axis pulse direction of the Non-bus servo is positive.
=1: The 2nd axis pulse direction of the Non-bus servo is negative.
PD2
=0: The 2nd axis pulse direction of the Non-bus servo is positive.
=1: The 3rd axis pulse direction of the Non-bus servo is negative.
PD3
=0: The 3rd axis pulse direction of the Non-bus servo is positive.
=1: The 4th axis pulse direction of the Non-bus servo is negative.
PD4
=0: The 4th axis pulse direction of the Non-bus servo is positive.
=1: The 5th axis pulse direction of the Non-bus servo is negative.
PD5
=0: The 5th axis pulse direction of the Non-bus servo is positive.
Standard setting：0 0 0 0 0 0 0 1
System parameter number
0
1
SCBM
0
RCUR
MSL
RLC
ZCL
SCBM
=1: Perform the stroke detection before moving.
=0: Do not perform the stroke detection before moving.
ZCL
=1: Clear the relative coordinate of the reference point return.
=0: Do not clear the relative coordinate of the reference point return.
350
Appendix One GSK218MC Parameter List
=1: Cancel the relative coordinate after resetting.
RLC
=0: Do not cancel the relative coordinate after resetting.
=1: The start line is the one which cursor locates when circularly starting the
MSL
multi-block MDI.
=0: The start line is the first line of the program when circularly starting the
multi-block MDI.
=1: Non-editing mode resetting cursor returns to the start position of the
RCUR
program.
=0: Non-editing mode resetting cursor does not return to the start position of
the program.
Standard setting：0 0 0 0 0 0 1 0
System parameter number
0
1
1
BFA
LZR
OUT2
=1: Prohibit entering the external area of the 2nd stroke limit.
OUT2
=0: Prohibit entering the internal area of the 2nd stroke limit.
=1: Perform the stroke detection after the power is turned on till to the manual
LZR
reference point return.
=0: Do not perform the stroke detection after the power is turned on till to the
manual reference point return.
=1: The alarm occurs followed with the overtravel when the overtravel code
BFA
APPEDIX
issues.
=0: The alarm occurs before the overtravel when the overtravel code issues.
(System alarm range is previous 5mm of each boundary for the prohibition
area)
Standard setting：0 0 0 0 0 0 0 1
System parameter number
0
1
RPD
2
RDR
FDR
TDR
RFO
LRP
RPD
=1: Manual rapid is enabled from the power-on till to the reference point return.
=0: Manual rapid is disabled from the power-on till to the reference point return.
LRP
=1: Positioning (G00) interpolation type is straight line.
=0: Positioning (G00) interpolation type is non-straight line.
RFO
=1: Rapid feed, it stops when the feedrate is Fo.
=0: Rapid feed, it does not stop when the feedrate is Fo.
TDR
=1: During the tapping, the dry run is enabled.
=0: During the tapping, the dry run is disabled.
FDR
=1: The dry run is enabled during cutting feed.
351
GSK218MC Series Machining Center CNC System Programming & Operation Manual
=0: The dry run is disabled during cutting feed.
=1: The dry run is enabled in the rapid positioning.
RDR
=0: The dry run is disabled in the rapid positioning.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
1
3
HPC
NPC
=1: The feed/rev. is enabled when the position encoder does not install.
NPC
=0: The feed/rev. is disabled when the position encoder does not install.
=1: System installs a position encoder.
HPC
=0: System does not install a position encoder.
Standard setting：0 0 0 0 0 0 1 0
System parameter number
0
1
4
DLF
=1: Manual zero return positions to the reference point manually at the rapid
DLF
traverse rate after the refernce point establishes and memories.
=0: Manual zero return positions to the reference point at the rapid traverse
rate after the refernce point establishes and memories.
Standard setting：0 0 0 0 0 0 0 0
APPEDIX
System parameter number
0
1
STL
5
PIIS
PPCK
ASL
PLAC
STL
=1: Select the pre-reading machining method.
=0: Select the non-pre-reading machining method.
PLAC
=1: The acceleration/deceleration method after the predictive control
interpolation: Exponent type.
=0: The acceleration/deceleration method after the predictive control
interpolation: Linear type.
ASL
=1: The automatic corner deceleration function of the predictive control:
Velocity difference control.
=0: The automatic corner deceleration function of the predictive control: Angle
control.
PPCK
=1: Predictive control performs the in-position detection.
=0: Predictive control do not perform the in-position detection.
PIIS
352
=1: The overlapping interpolation of acceleration/deceleration block is enabled
before the predictive control.
Appendix One GSK218MC Parameter List
=0: The overlapping interpolation of acceleration/deceleration block is disabled
before the predictive control.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
1
6
ALS
FLLS
FBLS
FBOL
=1: Rapid operation mode: Backward acceleration/deceleration.
FBOL
=0: Rapid operation mode: Forward acceleration/deceleration.
=1: The acceleration/deceleration before the rapid traverse: S type.
FBLS
=0: The acceleration/deceleration before the rapid traverse: Linear type.
=1: The acceleration/deceleration after the rapid traverse: Exponent type.
FLLS
=0: The acceleration/deceleration after the rapid traverse: Linear type.
=1: Automatic corner feed function is enabled.
ALS
=1: Automatic corner feed function is disabled.
Standard setting：0 0 0 0 0 0 1 0
System parameter number
0
1
7
CPCT
CALT
WLOE
HLOE
CLLE
CBLS
CBOL
=1: Cutting feed mode: Backward acceleration/deceleration.
CBOL
=0: Cutting feed mode: Forward acceleration/deceleration.
=1: The acceleration/deceleration before the cutting feed: S type.
CBLS
APPEDIX
=0: The acceleration/deceleration before the cutting feed: Linear type.
=1: The acceleration/deceleration after the cutting feed: Exponent type.
CLLE
=1: The acceleration/deceleration after the cutting feed: Linear type.
=1: JOG operation selection: Exponent type.
HLOE
=0: JOG operation selection: Linear type.
=1: MPG operation selection: Exponent type.
WLOE
=0: MPG operation selection: Linear type.
=1: Cutting feed acceleration clamping.
CALT
=0: Cutting feed acceleration releasing.
=1: Cutting feed controls the in-position accuracy.
CPCT
=0: Cutting feed does not control the in-position accuracy.
Standard setting：1 0 1 0 0 0 0 1
System parameter number
0
1
RVIT
8
RVCS
RBK
RVIT
=1: The next block is performed after the compensation is performed when the
353
GSK218MC Series Machining Center CNC System Programming & Operation Manual
reverse interval is more than the interval allowable tolerance D-value.
=0: The next block is performed after the compensation does not perform when
the reverse interval is more than the interval allowable tolerance D-value.
=1: The cutting feed/rapid movement is separately performed the interval
RBK
compensatin.
=0: The cutting feed/rapid movement does not separately perform the interval
compensatin.
=1: Reverse interval compensation mode: Speed-up/speed-down.
RVCS
=0: Reverse interval compensation mode: Fixed frequency.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
1
9
ALMS
ALM5
ALM4
ALM3
ALM2
ALM1
=1: The alarm is generated when the 1st axis drive alarm signal is set to 1.
ALM1
=0: The alarm is generated when the 1st axis drive alarm signal is set to 0.
=1: The alarm is generated when the 2nd axis drive alarm signal is set to 1.
ALM2
=0: The alarm is generated when the 2nd axis drive alarm signal is set to 0.
=1: The alarm is generated when the 3rd axis drive alarm signal is set to 1.
ALM3
=0: The alarm is generated when the 3rd axis drive alarm signal is set to 0.
=1: The alarm is generated when the 4th axis drive alarm signal is set to 1.
ALM4
=0: The alarm is generated when the 4th axis drive alarm signal is set to 0.
=1: The alarm is generated when the 5th axis drive alarm signal is set to 1.
APPEDIX
ALM5
=0: The alarm is generated when the 5th axis drive alarm signal is set to 0.
=1: The alarm is generated when the spindle drive alarm signal is set to 1.
ALMS
=0: The alarm is generated when the spindle drive alarm signal is set to 0.
Standard setting：0 0 1 0 0 0 0 0
System parameter number
0
2
ITL
0
UHSM
APC
MAPC
ZRS
=1: The interlocking of the overall axes are enabled.
=0: The interlocking of the overall axes are disabled.
ZRS
=1: The zero point signal is subject on the machine coordinate.
=0: The zero point signal is subject on the absolute encoder.
MAPC
=1: Select the absolute encoder: Multi-coil.
=0: Select the absolute encoder: Single-coil.
APC
=1: Use an absolute encoder.
=0: Do not use an absolute encoder.
UHSM
354
=1: Directly set the machine zero by manual.
ITL
Appendix One GSK218MC Parameter List
=0: The machine zero can not be directly set by manual.
Standard setting：1 0 0 0 0 0 0 0
System parameter number
0
2
1
APZ5
APZ4
APZ3
APZ2
APZ1
=1: The current machine position of the 1st axis sets to zero.
APZ1
=0: The current machine position of the 1st axis does not set to zero.
=1: The current machine position of the 2nd axis sets to zero.
APZ2
=0: The current machine position of the 2nd axis does not set to zero.
=1: The current machine position of the 3rd axis sets to zero.
APZ3
=0: The current machine position of the 3rd axis does not set to zero.
=1: The current machine position of the 4th axis sets to zero.
APZ4
=0: The current machine position of the 4th axis does not set to zero.
=1: The current machine position of the 5th axis sets to zero.
APZ5
=0: The current machine position of the 5th axis does not set to zero.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
2
2
DAL
=1: The absolute position display considers the tool length compensation.
DAL
=0: The absolute position display does not consider the tool length
APPEDIX
compensation.
Standard setting：0 0 0 0 0 0 0
System parameter number
0
2
3
POSM
=1: Program monitoring page displays the modal.
POSM
=0: Program monitoring page does not display the modal.
Standard setting：0 1 0 0 0 0 0 0
System parameter number
0
2
NPA
4
NPA
=1: Shift to the alarm screen when alarm issues.
=0: Do not shift to the alarm screen when alarm issues.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
355
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0
2
5
ALM
DGN
GRA
SET
SYS
PRG
POS
=1: In the position interface, shift the screen by pressing the “Position” button
POS
again.
=0: In the position interface, do not shift the screen by pressing the “Position”
button again.
=1: In the position interface, shift the screen by pressing the “Program” button
PRG
again.
=0: In the position interface, do not shift the screen by pressing the “Program”
button again.
=1: In the position interface, shift the screen by pressing the “System” button
SYS
again.
=0: In the position interface, do not shift the screen by pressing the “System”
button again.
=1: In the position interface, shift the screen by pressing the “Setting” button
SET
again.
=0: In the position interface, do not shift the screen by pressing the “Setting”
button again.
=1: In the position interface, shift the screen by pressing the “Graph” button
GRA
again.
=0: In the position interface, do not shift the screen by pressing the “Graph”
button again.
APPEDIX
=1: In the position interface, shift the screen by pressing the “Diagnosis” button
DGN
again.
=0: In the position interface, do not shift the screen by pressing the “Diagnosis”
button again.
=1: In the position interface, shift the screen by pressing the “Alarm” button
ALM
again.
=0: In the position interface, do not shift the screen by pressing the “Alarm”
button again.
Standard setting：1 1 1 1 0 1 1 1
System parameter number
0
2
PETP
6
HELP
PLC
SMDT
SMDI
SPET PETP
=1: Automatically skip to the program page by “Editing” button.
=0: Do not automatically skip to the program page by “Editing” button.
SPET
356
=1: In the Editing mode, automatically skip to the program interface by
<PROGRAM>.
Appendix One GSK218MC Parameter List
=0: In the Editing mode, do not automatically skip to the program interface by
<PROGRAM>.
=1: In the MDI mode, automatically skip to the MDI interface by <PROGRAM>.
SMDI
=0: In the MDI mode, do not automatically skip to the MDI interface by
<PROGRAM>.
=1: In the MDI mode, automatically skip th the CUR/MOD interface selection.
SMDT
=0: In the MDI mode, automatically skip th the MDI interface selection.
=1: In the PLC interface, shift the page by pressing the “Program control”
PLC
button again.
=0: In the PLC interface, do not shift the page by pressing the “Program
control” button again.
=1: In the Help interface, shift the screen by pressing the “Help” button again.
HELP
=0: In the Help interface, do not shift the screen by pressing the “Help” button
again.
Standard setting：1 1 0 0 0 0 0 1
System parameter number
0
2
7
NE9
NE8
=1: Prohibit the sub-program editing of the program numbers 80000 – 89999.
NE8
=0: Allow the sub-program editing of the program numbers 80000 – 89999.
=1: Prohibit the sub-program editing of the program numbers 90000 - 99999.
NE9
APPEDIX
=0: Allow the sub-program editing of the program numbers 90000 - 99999.
Standard setting：0 0 0 1 0 0 0 1
System parameter number
0
2
8
MCL
MKP
=1: Clear the compiled program when performing the M02, M30 or % in the
MKP
MDI mode.
=1: Keep the compiled program when performing the M02, M30 or % in the
MDI mode.
=1: Delete the compiled program by resetting button in MDI mode.
MCL
=0: Retain the compiled program by resetting button in MDI mode.
Standard setting：0 0 0 1 0 0 0 0
System parameter number
0
2
WOF
9
IWZ
WZO
MCV
GOF
WOF
=1: Prohibit inputting the tool wear offset value by MDI keyboard.
357
GSK218MC Series Machining Center CNC System Programming & Operation Manual
=0: Input the tool wear offset value by MDI keyboard.
=1: Prohibit inputting the tool geometry offset value by MDI keyboard.
GOF
=0: Input the geometry offset value by MDI keyboard.
=1: Prohibit inputting the macro program varible by MDI keyboard.
MCV
=0: Input the macro program variable by MDI keyboard.
=1: Prohibit inputting the workpiece origin offset value by MDI keyboard.
WZO
=0: Input the workpiece origin offset value by MDI keyboard
=1: Prohibit inputting the workpiece origin offset value by MDI keyboard in the
IWZ
dwell.
=0: Input the workpiece origin offset value by MDI keyboard in the dwell.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
3
1
G13
G91
G19
G18
G01
=1: It is the G01 mode when the power is turned on or the state is cleared.
G01
=0: It is the G00 mode when the power is turned on or the state is cleared.
=1: The plane selection is G18 mode when the power is turned on or the state
G18
is cleared.
=0: The plane selection is G17 mode when the power is turned on or the state
is cleared.
=1: It is the G19 mode, when G19=1, it is better set the G18 to 0.
G19
APPEDIX
=0: It is determined by bit 1 of parameter No.:31.
G19
G18
G17, G18 and G19 methods
0
0
G17 method (X-Y plane)
0
1
G18 method (Z-X plane)
1
0
G19 method (Y-Z plane)
=1: It sets to the G91 mode when the power is turned on or the state is cleared.
G91
=0: It sets to the G90 mode when the power is turned on or the state is cleared.
=1: It sets to the G13 mode when the power is turned on or the state is cleared.
G13
=0: It sets to the G12 mode when the power is turned on or the state is cleared.
Standard setting：0 0 1 0 0 0 0 0
System parameter number
0
3
AD2
358
2
AD2
=1: Specify two or more same addresses in a same block, the system then
alarms.
Appendix One GSK218MC Parameter List
=0: Specify two or more same addresses in a same block, the system does not
alarms.
Standard setting：0 1 0 0 0 0 0 0
System parameter number
0
3
3
M3B
M30
M02
=1: Return to the start of the block when performing to the M02.
M02
=0: Do not return to the start of the block when performing to the M02.
=1: Return to the start of the block when performing to the M30.
M30
=0: Return to the start of the block when performing to the M30.
=1: Up to 3 M codes can be specified in a program.
M3B
=0: Only one M code can be specified in a program.
Standard setting：1 0 0 1 0 0 0 0
System parameter number
0
3
4
CFH
DWL
=1: In the feed/rev. mode, G04 is the dwell of per revelution.
DWL
=0: In the feed/rev. mode, G04 is not the dwell of per revelution.
=1: Clear the F, H and D codes when resetting or ESP.
CFH
=0: Remain the F, H and D codes when resetting or ESP.
Standard setting：0 0 0 0 0 0 0 0
APPEDIX
System parameter number
0
3
C01
5
C07
C06
C05
C04
C03
C02
C01
=1: Clear the G codes in group 01 when resetting or ESP.
=0: Reserve the G codes in group 01 when resetting or ESP.
C02
=1: Clear the G codes in group 02 when resetting or ESP.
=0: Reserve the G codes in group 02 when resetting or ESP.
C03
=1: Clear the G codes in group 03 when resetting or ESP.
=0: Reserve the G codes in group 03 when resetting or ESP.
C04
=1: Clear the G codes in group 04 when resetting or ESP.
=0: Reserve the G codes in group 04 when resetting or ESP.
C05
=1: Clear the G codes in group 05 when resetting or ESP.
=0: Reserve the G codes in group 05 when resetting or ESP.
C06
=1: Clear the G codes in group 06 when resetting or ESP.
=0: Reserve the G codes in group 06 when resetting or ESP.
C07
=1: Clear the G codes in group 07 when resetting or ESP.
359
GSK218MC Series Machining Center CNC System Programming & Operation Manual
=0: Reserve the G codes in group 07 when resetting or ESP.
Standard setting：1 0 0 0 0 0 0 0
System parameter number
0
3
6
C15
C14
C13
C12
C11
C10
C09
C08
BDP
SCRW
=1: Clear the G codes in group 08 when resetting or ESP.
C08
=0: Reserve the G codes in group 08 when resetting or ESP.
=1: Clear the G codes in group 09 when resetting or ESP.
C09
=0: Reserve the G codes in group 09 when resetting or ESP.
=1: Clear the G codes in group10 when resetting or ESP.
C10
=0: Reserve the G codes in group 10 when resetting or ESP.
=1: Clear the G codes in group 11 when resetting or ESP.
C11
=0: Reserve the G codes in group 11 when resetting or ESP.
=1: Clear the G codes in group 12 when resetting or ESP.
C12
=0: Reserve the G codes in group 12 when resetting or ESP.
=1: Clear the G codes in group 13 when resetting or ESP.
C13
=0: Reserve the G codes in group 13when resetting or ESP.
=1: Clear the G codes in group 14 when resetting or ESP.
C14
=0: Reserve the G codes in group 14 when resetting or ESP.
=1: Clear the G codes in group 15 when resetting or ESP.
C15
=0: Reserve the G codes in group 15 when resetting or ESP.
APPEDIX
Standard setting：0 0 0 0 0 0 0 1
System parameter number
0
3
SCRW
7
SOC
RSC
=1: Perform the pitch compensation.
=0: Do not perform the pitch compensation.
BDP
=1: Use the bi-directional pitch error compensation.
=0: Do not use the bi-directional pitch error compensation.
RSC
=1: Calculating the reference coordinate of G96 spindle speed is regarded as
current point when the G0 is positioned at the rapid traverse rate.
=0: Calculating the reference coordinate of G96 spindle speed is regarded as
en point when the G0 is positioned at the rapid traverse rate.
SOC
=1: G96 spindle speed clamps after the spindle override.
=0: G96 spindle speed clamps before the spindle override.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
360
Appendix One GSK218MC Parameter List
0
3
8
PG2
PG1
FLRE
FLR
SAR
=1: Detect the spindle speed arrival signal.
SAR
=0: Do not detect the spindle speed arrival signal.
=1: In the spindle speed fluctuation check, the unit both the allowable rate (q)
FLR
and fluctuation rate (r) is 0.1%.
=0: In the spindle speed fluctuation check, the unit both the allowable rate (q)
and fluctuation rate (r) is 1%.
=1: Spindle speed fluctuation check is enabled.
FLRE
=1: Spindle speed fluctuation check is disabled.
PG2, PG1: The gear ratio between the spindle and position encoder. 00 is 1:1; 01 is 2:1;
10 is 4:1 and 11 is 8:1.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
3
9
TLC
=1: Select the type of the tool length compensation: Type B.
TLC
=0: Select the type of the tool length compensation: Type A.
Standard setting：0 0 0 0 0 0 0 1
System parameter number
0
4
0
ODI
CCN
SUP
APPEDIX
=1: The start type in the cutter compensation: Type B.
SUP
=0: The start type in the cutter compensation: Type A.
=1: G28, G30 commands are moved to the intermediate point, and then cancel
CCN
the radius compensation.
=0: G28, G30 commands are moved to the intermediate point, and then retain
the radius compensation.
=1: Set the cutter compensation value based upon its diameter value.
ODI
=0: Set the cutter compensation value based upon its radius value.
Standard setting：1 0 0 0 0 1 0 0
System parameter number
0
4
PUIT
1
CNI
G39
PUIT
=1: The input and display of the data parameter are determined by bit
parameter NO.0#2 INI.
=0: The input and display of the data parameter are metric system.
361
GSK218MC Series Machining Center CNC System Programming & Operation Manual
=1: In the radius compensation, the corner arc function is enabled.
G39
=0: In the radius compensation, the corner arc function is disabled.
=1: Radius compensation performs the interference inspection.
CNI
=0: Radius compensation does not perform the interference inspection.
Standard setting：0 1 1 0 0 0 0 0
System parameter number
0
4
2
RD2
RD1
=1: Set the tool-retraction direction of G76, G87: Negative.
RD1
=0: Set the tool-retraction direction of G76, G87: Positive.
=1: Set the tool-retraction axis of the G76, G87: The 2nd axis.
RD2
=0: Set the tool-retraction axis of the G76, G87: The 1st axis.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
4
3
QZA
=1: In the peck drilling (G73, G83), the alarm will generate if the cutting value
QZA
does not specify.
=0: In the peck drilling (G73, G83), the alarm will not generate even if the
cutting value does not specify.
Standard setting：0 0 0 0 0 0 1 0
APPEDIX
System parameter number
0
4
4
PCP
DOV
VGR
=1: The gear ratio between the spindle and position encoder can be set
VGR
arbitrarily.
=0: The gear ratio between the spindle and position encoder can not be set
freely.
=1: The override is enabled when the rigid tapping is performed the
DOV
tool-retraction.
=1: The override is disabled when the rigid tapping is performed the
tool-retraction.
=1: The tapping is the high-speed peck tapping cycle.
PCP
=0: The tapping is the standard peck tapping cycle.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
362
4
5
OVS
OVU
TDR
NIZ
Appendix One GSK218MC Parameter List
=1: Perform the rigid tapping smooth treatment.
NIZ
=0: Do not perform the rigid tapping smooth treatment.
=1: Rigid tapping in-feed. Use the identical time constante when tool-retraction
TDR
is performed.
=0: Rigid tapping in-feed. Do not use the identical time constante when
tool-retraction is performed.
=1: The unit of the rigid tapping tool-retraction override is 10%.
OVU
=0: The unit of the rigid tapping tool-retraction override is 1%.
=1: In the rigid tapping, the feedrate selection and override cancellation signal
OVS
are enabled.
=0: In the rigid tapping, the feedrate selection and override cancellation signal
are disabled.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
4
6
ORI
SSOG
=1: At the beginning of the tapping, the control method of spindle is servo.
SSOG
=0: At the beginning of the tapping, the control method of spindle is follow.
=1: At the beginning of the tapping, the spindle dwells.
ORI
=0: At the beginning of the tapping, the spindle does not dwell.
APPEDIX
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
4
RIN
7
XSC
SCL3
SCL2
SCL1
RIN
=1: The rotation angle of the coordinate rotation: G90/G91 command.
=0: The rotation angle of the coordinate rotation: Absolute command.
SCL1
=1: The scaling of the 1st axis is enabled.
=0: The scaling of the 1st axis is disabled.
SCL2
=1: The scaling of the 2nd axis is enabled.
=0: The scaling of the 2nd axis is disabled.
SCL3
=1: The scaling of the 3rd axis is enabled.
=0: The scaling of the 3rd axis is disabled.
XSC
=1: The specification method of the scaling override along each axis is I, J or K.
=0: The specification method of the scaling override along each axis is P code.
Standard setting：0 1 1 1 1 0 0 1
System parameter number
363
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0
4
8
MDL
=1: The unidirectional position G code is set to modal code.
MDL
=0 : The unidirectional position G code does not set to modal code.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
4
9
RPST
=1: Z axis moves with the G01 mode during the restart of program.
RPST
=0: Z axis moves at the dry run speed with the G00 mode during the restart of
program.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
0
SIM
G90
REL
=1: The relative display setting of the index worktable: Within 360°.
REL
=0 : The relative display setting of the index worktable: Without 360°.
=1: Index command: Absolute command.
G90
=0: Index command: G90/G91 command.
=1: The alarm occurs when the index code and other controllable axis codes
SIM
are share with a same block.
APPEDIX
=0: The alarm does not occur when the index code and other controllable axis
codes are share with a same block.
Standard setting：0 1 0 0 0 0 0 0
System parameter number
0
5
1
MDLY
SBM
=1: The single block can be used in the macro program command statement.
SBM
=0: The single block can not be used in the macro program command
statement.
=1: Without delay in the macro program command statement.
MDLY
=1: Delays in the macro program command statement.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
CCV
364
2
CLV
CCV
=1: Macro program common variables #100 - #199 will be cleared after
Appendix One GSK218MC Parameter List
resetting.
=0: Macro program common variables #100 - #199 will not be cleared after
resetting.
=1: Macro program local variables #1 - #50 will be cleared after resetting.
CLV
=0: Macro program local variables #1 - #50 will not be cleared after resetting.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
3
PLCV
LAD0~LAD3
LAD3
LDA2
LAD1
LAD0
are the binary combination parameter. Use the No.0 ladder digram when it
is set to 0; Use the No. 0~15 ladder diagrams when it set to 1~15.
=1: Read and display the PLC software version number.
PLCV
=0: Do not read and display the PLC software version number.
Standard setting：1 0 0 0 0 0 0 1
System parameter number
0
5
4
OPRG
=1: One-touch input/output is enabled to the component program when
OPRG
performing the debugging or its above authority.
=0: One-touch input/output is disabled to the component program when
performing the debugging or its above authority.
APPEDIX
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
5
CANT
=1: Single machining time is automatically cleared.
CANT
=0: Single machining time is not automatically cleared.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
HPF
6
HNGD
HISR
HPF
=1: MPG movement amount selects the absolutely operation.
=0: MPG movement amount does not select the absolutely operation.
HISR
=1: Use the MPG/single-step interruption function.
=0: Do not use the MPG/single-step interruption function.
HNGD
=1: The movement along each axis is identical with the MPG revolving
direction.
365
GSK218MC Series Machining Center CNC System Programming & Operation Manual
=0: The movement along each axis is different with the MPG revolving
direction.
Standard setting：1 0 0 0 0 0 0 1
System parameter number
0
5
7
PLW5
PLW4
PLW3
PLW2
PLW1
=1: The 1st axis pulse width changes along with the speed.
PLW1
=0: The 1st axis pulse width fixes at 1ms.
=1: The 2nd axis pulse width changes along with the speed.
PLW2
=0: The 2nd axis pulse width fixes at 1ms.
=1: The 3rd axis pulse width changes along with the speed.
PLW3
=0: The 3rd axis pulse width fixes at 1ms.
=1: The 4th axis pulse width changes along with the speed.
PLW4
=0: The 4th axis pulse width fixes at 1ms.
=1: The 5th axis pulse width changes along with the speed.
PLW5
=0: The 5th axis pulse width fixes at 1ms.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
5
9
LEDT
LOPT
RHPG
=1: Use the electric MPG drive function.
RHPG
APPEDIX
=0: Do not use the electric MPG drive function.
=1: Operation panel locking singal is enabled.
LOPT
=0: Operation panel locking singal is disabled.
=1: External program locking signal is enabled.
LEDT
=0: External program locking signal is disabled.
Standard setting：0 0 0 0 0 0 0 0
System parameter number
0
6
0
SCL
EPW
=1: The Max. quantity of the position switches are 16.
EPW
=0: The Max. quantity of the position switches are 10.
=1: Use the scaling.
SCL
=0: Do not use the scaling.
Standard setting：0 0 1 0 0 0 0 0
System parameter number
0
366
6
1
FALM
LALM
EALM
SALM
AALM
SSC
Appendix One GSK218MC Parameter List
SSC
=1: Use the constant peripheral speed control.
=0: Do not use the constant peripheral speed control.
AALM
=1: Ignor external user alarm.
=1: Do not ignore external user alarm.
SALM
=1: Ignore the spindle drive alarm.
=0: Do not ignore the spindle drive alarm.
EALM
=1: Ignore the ESP alarm.
=0: Do not ignore ESP alarm.
LALM
=1: Ignore hard-limit alarm.
=0: Do not ignore hard-limit alarm.
FALM
=1: Ignore feed axis drive alarm.
=0: Do not ignore feed axis drive alarm.
Standard setting：0 0 0 0 0 0 0 0
APPEDIX
367
GSK218MC Series Machining Center CNC System Programming & Operation Manual
2.
Data Parameter
Parameter No.
0000
Parameter definition
Default value
I/O channel, input/output equipment
2
(0:Xon/Xoff 1:XModem 2:USB)
Setting range：0～2
When CNC is performed the communication with the PC machine by the RS232 interface, set it as
the 0 or 1, and it is set to 2 when connecting with the U disk.
0001
Communication channel Baud Rate (DNC)
38400
Setting range：0～115200 （Unit：BPS）
0002
Communication channel Baud Rate (Transmission
115200
file)
Setting range：0～115200 （Unit：BPS）
0004
System interporlation period (1, 2, 4, and 8ms)
1
Setting range：1～8
APPEDIX
0005
CNC controllable axis number
4
Setting range：3～5
0006
System language selection
Setting range：0～3
0008
0: Chinese
1: English
0
2: Russian
3: Spanish
The dimension of the slave state MDT data package
12
of the Ethernet bus
Setting range：0～20
0009
The Max. retransmission times of the Ethernet bus
10
Setting range：0～30
0010
The 1st axis offset value of the external workpiece
origin
Setting range：-9999.9999～9999.9999（mm)
368
0.0000
Appendix One GSK218MC Parameter List
0011
The 2nd axis offset value of the external workpiece
0.0000
origin
Setting range：-9999.9999～9999.9999（mm)
0012
The 3rd axis offset value of the external workpiece
0.0000
origin
Setting range：-9999.9999～9999.9999（mm)
0013
The 4th axis offset value of the external workpiece
0.0000
origin
Setting range：-9999.9999～9999.9999（mm)
0014
The 5th axis offset value of the external workpiece
0.0000
origin
Setting range：-9999.9999～9999.9999（mm)
0015
The 1st axis workpiece origin offset value of G54
0.0000
Setting range：-9999.9999～9999.9999（mm）
The 2nd axis workpiece origin offset value of G54
0.0000
APPEDIX
0016
Setting range：-9999.9999～9999.9999（mm）
0017
The 3rd axis workpiece origin offset value of G54
0.0000
Setting range：-9999.9999～9999.9999（mm）
0018
The 4th axis workpiece origin offset value of G54
0.0000
Setting range：-9999.9999～9999.9999（mm）
0019
The 5th axis workpiece origin offset value of G54
0.0000
Setting range：-9999.9999～9999.9999（mm）
0020
The 1st axis workpiece origin offset value of G55
0.0000
Setting range：-9999.9999～9999.9999（mm）
0021
The 2nd axis workpiece origin offset value of G55
0.0000
369
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Setting range：-9999.9999～9999.9999（mm）
0022
The 3rd axis workpiece origin offset value of G55
0.0000
Setting range：-9999.9999～9999.9999（mm）
0023
The 4th axis workpiece origin offset value of G55
0.0000
Setting range：-9999.9999～9999.9999（mm）
0024
The 5th axis workpiece origin offset value of G55
0.0000
Setting range：-9999.9999～9999.9999（mm）
0025
The 1st axis workpiece origin offset value of G56
0.0000
Setting range：-9999.9999～9999.9999（mm）
0026
The 2nd axis workpiece origin offset value of G56
0.0000
Setting range：-9999.9999～9999.9999（mm）
0027
The 3rd axis workpiece origin offset value of G56
0.0000
Setting range：-9999.9999～9999.9999（mm）
APPEDIX
0028
The 4th axis workpiece origin offset value of G56
0.0000
Setting range：-9999.9999～9999.9999（mm）
0029
The 5th axis workpiece origin offset value of G56
0.0000
Setting range：-9999.9999～9999.9999（mm）
0030
The 1st axis workpiece origin offset value of G57
0.0000
Setting range：-9999.9999～9999.9999（mm）
0031
The 2nd axis workpiece origin offset value of G57
0.0000
Setting range：-9999.9999～9999.9999（mm）
0032
The 3rd axis workpiece origin offset value of G57
Setting range：-9999.9999～9999.9999（mm）
370
0.0000
Appendix One GSK218MC Parameter List
0033
The 4th axis workpiece origin offset value of G57
0.0000
Setting range：-9999.9999～9999.9999（mm）
0034
The 5th axis workpiece origin offset value of G57
0.0000
Setting range：-9999.9999～9999.9999（mm）
0035
The 1st axis workpiece origin offset value of G58
0.0000
Setting range：-9999.9999～9999.9999（mm）
0036
The 2nd axis workpiece origin offset value of G58
0.0000
Setting range：-9999.9999～9999.9999（mm）
0037
The 3rd axis workpiece origin offset value of G58
0.0000
Setting range：-9999.9999～9999.9999（mm）
0038
The 4th axis workpiece origin offset value of G58
0.0000
Setting range：-9999.9999～9999.9999（mm）
0039
The 5th axis workpiece origin offset value of G58
0.0000
Setting range：-9999.9999～9999.9999（mm）
The 1st axis workpiece origin offset value of G59
APPEDIX
0040
0.0000
Setting range：-9999.9999～9999.9999（mm）
0041
The 2nd axis workpiece origin offset value of G59
0.0000
Setting range：-9999.9999～9999.9999（mm）
0042
The 3rd axis workpiece origin offset value of G59
0.0000
Setting range：-9999.9999～9999.9999（mm）
0043
The 4th axis workpiece origin offset value of G59
0.0000
Setting range：-9999.9999～9999.9999（mm）
0044
The 5th axis workpiece origin offset value of G59
0.0000
Setting range：-9999.9999～9999.9999（mm）
371
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0045
The 1st axis coordinate value of the 1st reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0046
The 2nd axis coordinate value of the 1st reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0047
The 3rd axis coordinate value of the 1st reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0048
The 4th axis coordinate value of the 1st reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0049
The 5th axis coordinate value of the 1st reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
APPEDIX
0050
The 1st axis coordinate value of the 2nd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0051
The 2nd axis coordinate value of the 2nd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0052
The 3rd axis coordinate value of the 3rd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0053
The 4th axis coordinate value of the 2nd reference
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
372
0.0000
Appendix One GSK218MC Parameter List
0054
The 2nd axis coordinate value of the 5th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0055
The 1st axis coordinate value of the 3rd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0056
The 2nd axis coordinate value of the 3rd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm)
0057
The 3rd axis coordinate value of the 3rd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0058
The 4th axis coordinate value of the 3rd reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
The 5th axis coordinate value of the 3rd reference
0.0000
APPEDIX
0059
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0060
The 1st axis coordinate value of the 4th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm）
0061
The 2nd axis coordinate value of the 4th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm)
0062
The 3rd axis coordinate value of the 4th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm)
373
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0063
The 4th axis coordinate value of the 4th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm)
0064
The 5th axis coordinate value of the 4th reference
0.0000
point on the mechanical coordinate system
Setting range：-9999.9999～9999.9999（mm)
0066
The coordinate value of the stored stroke detection 1
-9999
st
along the reverse boundary of the 1 axis
Setting range：-9999.9999～9999.9999（mm)
0067
The coordinate value of the stored stroke detection 1
9999
along the positive boundary of the 1st axis
Setting range：-9999.9999～9999.9999（mm)
0068
The coordinate value of the stored stroke detection 1
nd
along the reverse boundary of the 2
-9999
axis
Setting range：-9999.9999～9999.9999（mm)
APPEDIX
0069
The coordinate value of the stored stroke detection 1
9999
along the positive boundary of the 2nd axis
Setting range：-9999.9999～9999.9999（mm)
0070
The coordinate value of the stored stroke detection 1
-9999
rd
along the reverse boundary of the 3 xis
Setting range：-9999.9999～9999.9999（mm)
0071
The coordinate value of the stored stroke detection 1
9999
rd
along the positive boundary of the 3 axis
Setting range：-9999.9999～9999.9999（mm)
0072
The coordinate value of the stored stroke detection 1
th
along the reverse boundary of the 4 axis
Setting range：-9999.9999～9999.9999（mm)
374
-9999
Appendix One GSK218MC Parameter List
0073
The coordinate value of the stored stroke detection 1
9999
th
along the positive boundary of the 4 axis
Setting range：-9999.9999～9999.9999（mm)
0074
The coordinate value of the stored stroke detection 1
-9999
along the reverse boundary of the 5th axis
Setting range：-9999.9999～9999.9999（mm)
0075
The coordinate value of the stored stroke detection 1
9999
th
along the positive boundary of the 5 axis
Setting range：-9999.9999～9999.9999（mm)
0076
The coordinate value of the stored stroke detection 2
-9999
along the reverse boundary of the 1st axis
Setting range：-9999.9999～9999.9999（mm)
0077
The coordinate value of the stored stroke detection 2
9999
st
along the positive boundary of the 1 axis
Setting range：-9999.9999～9999.9999（mm)
The coordinate value of the stored stroke detection 2
-9999
APPEDIX
0078
along the reverse boundary of the 2nd axis
Setting range：-9999.9999～9999.9999（mm)
0079
The coordinate value of the stored stroke detection 2
nd
along the positive boundary of the 2
9999
axis
Setting range：-9999.9999～9999.9999（mm)
0080
The coordinate value of the stored stroke detection 2
-9999
rd
along the reverse boundary of the 3 axis
Setting range：-9999.9999～9999.9999（mm)
0081
The coordinate value of the stored stroke detection 2
nd
along the positive boundary of the 2
9999
axis
Setting range：-9999.9999～9999.9999（mm)
375
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0082
The coordinate value of the stored stroke detection 2
-9999
th
along the reverse boundary of the 4 axis
Setting range：-9999.9999～9999.9999（mm)
0083
The coordinate value of the stored stroke detection 2
9999
along the positive boundary of the 4th axis
Setting range：-9999.9999～9999.9999（mm)
0084
The coordinate value of the stored stroke detection 2
-9999
th
along the reverse boundary of the 5 axis
Setting range：-9999.9999～9999.9999（mm)
0085
The coordinate value of the stored stroke detection 2
9999
along the positive boundary of the 5th axis
Setting range：-9999.9999～9999.9999（mm)
0086
Dry run speed
5000
Setting range：0～9999 (mm/min)
0087
The cutting feedrate when the power is turned on.
300
APPEDIX
Setting range：0～9999 (mm/min)
0088
G0 rapid traverse rate along the 1st axis
5000
Setting range：
Metric: 0～30000 (mm/min)
Inch: 0～30000/ 25.4（inch/min）
Rotation axis: 0～30000（deg/min）
0089
G0 rapid traverse rate along the 2nd axis
5000
Setting range：
Metric: 0～30000 (mm/min)
Inch: 0～30000/ 25.4（inch/min）
Rotation axis: 0～30000（deg/min）
0090
G0 rapid traverse rate along the 3rd axis
Setting range：
Metric: 0～30000 (mm/min)
376
5000
Appendix One GSK218MC Parameter List
Inch: 0～30000/ 25.4（inch/min）
Rotation axis: 0～30000（deg/min）
0091
G0 rapid traverse rate along the 4th axis
5000
Setting range：
Metric: 0～30000 (mm/min)
Inch: 0～30000/ 25.4（inch/min）
Rotation axis: 0～30000（deg/min）
0092
G0 rapid traverse rate along the 5th axis
5000
Setting range：
Metric: 0～30000 (mm/min)
Inch: 0～30000/ 25.4（inch/min）
Rotation axis: 0～30000（deg/min）
0093
The Fo speed (General-purpose for overall axes) at
30
the rapid traverse rate along each axis
Setting range：0～1000 (mm/min)
0094
The top controllable speed (General-purpose for
8000
APPEDIX
overall axes) at the rapid position
Setting range：300～30000(mm/min)
0095
The lowest controllable speed (General-purpose for
0
overall axes) at the rapid position
Setting range：0～300 (mm/min)
0096
The top controllable speed (General-purpose for
6000
overall axes) for the cutting feed
Setting range：300～9999 (mm/min)
0097
The lowest controllable speed (General-purpose for
0
overall axes) for the cutting feed
Setting range：0～300 (mm/min)
0098
The consecutive feedrate of the JOG along each axis
2000
377
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Setting range：0～9999 (mm/min)
0099
(FL) speed (General-purpose for overall axes) when
40
gaining the Z pulse signal
Setting range：1～60 (mm/min)
0100
Reference position speed return along the 1st axis
4000
Setting range：0～9999 (mm/min)
0101
Reference position speed return along the 2nd axis
4000
Setting range：0～9999 (mm/min)
0102
Reference position speed return along the 3rd axis
4000
Setting range：0～9999 (mm/min)
0103
Reference position speed return along the 4th axis
4000
Setting range：0～9999 (mm/min)
0104
Reference position speed return along the 5th axis
4000
Setting range：0～9999 (mm/min)
APPEDIX
0105
Acceleration/deceleration
L-type
time
constant
100
constant
100
constant
100
constant
100
st
before the 1 axis at the rapid traverse rate
Setting range：3～400 （ms）
0106
Acceleration/deceleration
nd
before the 2
L-type
time
axis at the rapid traverse rate
Setting range：3～400 （ms）
0107
Acceleration/deceleration
L-type
time
rd
before the 3 axis at the rapid traverse rate
Setting range：3～400 （ms）
0108
Acceleration/deceleration
th
L-type
time
before the 4 axis at the rapid traverse rate
Setting range：3～400 （ms）
378
Appendix One GSK218MC Parameter List
0109
Acceleration/deceleration
L-type
time
constant
100
constant
100
constant
100
constant
100
constant
100
constant
100
Acceleration/deceleration L-type time constant after
80
th
before the 5 axis at the rapid traverse rate
Setting range：3～400 （ms）
0110
Acceleration/deceleration
S-type
time
st
before the 1 axis at the rapid traverse rate
Setting range：3～400 （ms）
0111
Acceleration/deceleration
S-type
time
before the 2nd axis at the rapid traverse rate
Setting range：3～400 （ms）
0112
Acceleration/deceleration
S-type
time
rd
before the 3 axis at the rapid traverse rate
Setting range：3～400 （ms）
0113
Acceleration/deceleration
S-type
time
before the 4th axis at the rapid traverse rate
Setting range：3～400 （ms）
Acceleration/deceleration
S-type
time
APPEDIX
0114
th
before the 5 axis at the rapid traverse rate
Setting range：3～400 （ms）
0115
st
the 1 axis at the rapid traverse rate
Setting range：0～400 （ms）
0116
Acceleration/deceleration L-type time constant after
nd
the 2
80
axis at the rapid traverse rate
Setting range：0～400 （ms）
0117
Acceleration/deceleration L-type time constant after
80
rd
the 3 axis at the rapid traverse rate
Setting range：0～400 （ms）
379
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0118
Acceleration/deceleration L-type time constant after
80
th
the 4 axis at the rapid traverse rate
Setting range：0～400 （ms）
0119
Acceleration/deceleration L-type time constant after
80
the 5th axis at the rapid traverse rate
Setting range：0～400 （ms）
0120
Acceleration/deceleration E-type time constant after
60
st
the 1 axis at the rapid traverse rate
Setting range：0～400 （ms）
0121
Acceleration/deceleration E-type time constant after
60
the 2nd axis at the rapid traverse rate
Setting range：0～400 （ms）
0122
Acceleration/deceleration E-type time constant after
60
rd
the 3 axis at the rapid traverse rate
Setting range：0～400 （ms）
APPEDIX
0123
Acceleration/deceleration E-type time constant after
60
the 4th axis at the rapid traverse rate
Setting range：0～400 （ms）
0124
Acceleration/deceleration E-type time constant after
60
th
the 5 axis at the rapid traverse rate
Setting range：0～400 （ms）
0125
Acceleration/deceleration
L-type
time
constant
100
S-type
time
constant
100
before the cutting feed
Setting range：3～400 （ms）
0126
Acceleration/deceleration
before the cutting feed
Setting range：3～400 （ms）
380
Appendix One GSK218MC Parameter List
0127
Acceleration/deceleration L-type time constant after
80
the cutting feed
Setting range：3～400 （ms）
0128
Acceleration/deceleration E-type time constant after
60
the cutting feed
Setting range：3～400 （ms）
0129
Acceleration/deceleration
FL
speed
of
the
10
Interpolate the Max. incorporative block numbers in
0
exponential type
Setting range：0～9999 （mm/min）
0130
adance
Setting range：0～10
0131
Cutting feed position accuracy
0.03
Setting range：0.001～0.5 （mm）
0132
Circular interpolation control accuracy
0.03
0133
Interpolate outline control accuracy in advance
APPEDIX
Setting range：0～0.5 （mm）
0.01
Setting range：0.01～0.5 （mm）
0134
The
acceleration
of
the
linear
250
acceleration/deceleration before interpolation in the
forecasting control method
Setting range：0～2000 （mm/s²）
0135
The acceleration/deceleration constent before S-type
100
in the forecasting control method.
Setting range：0～400 （ms）
0136
The linear acceleration/deceleration time constant
80
followed with the acceleration/deceleration in the
381
GSK218MC Series Machining Center CNC System Programming & Operation Manual
forecasting control.
Setting range：0～400 （ms）
0137
The
exponential
acceleration/deceleration
time
60
constant followed with the acceleration/deceleration
in the forecasting control.
Setting range：0～400 （ms）
0138
The exponential type acceleration/deceleration FL
10
speed of the cutting feed in forcasting control mode.
Setting range：0～400 （ms）
0139
Outline control accuracy of forcasting control mode.
0.01
Setting range：0～0.5 (mm)
0140
Merger block section in the forcasting control mode.
0
Setting range：0～10
0141
In-position accuracy in the forcasting control mode.
0.05
Setting range：0～0.5 (mm)
APPEDIX
0142
The condition for sampling length in the forcasting
5
control mode.
Setting range：0～30
0143
The condition for sampling angle in the forcasting
10
control mode.
Setting range：0～30
0144
The critical angle between two blocks of the
5
automatic corner deceleration in the forcasting
control mode.
Setting range：2～178
0145
(Degree)
The lowest feedrate of automatic corner deceleration
in the forcasting control mode
382
120
Appendix One GSK218MC Parameter List
Setting range：10～1000 (mm/min)
0146
The allowable error of each axis for the deceleration
80
function with the speed difference mode in the
forcasting control mode
Setting range：60～1000
0147
Cutting accuracy level in the forcasting control mode
2
Setting range：0～8
0148
The acceleration limit out of the circular arc
1000
interpolation
Setting range：100～5000 （mm/s²）
0149
The low speed lower-limit of the acceleration
200
clamping at the circular arc interpolation
Setting range：0～2000 (mm/min)
0150
The acceleration clamped time constant of the
50
cutting feed
0151
The Max. clamped speed in the MPG incomplete
APPEDIX
Setting range：0～1000（ms）
2000
operation mode
Setting range：0～3000
0152
(mm/min)
The linear acceleration/deceleration time constant of
120
MPG
Setting range：0～400 （ms）
0153
The
exponential
acceleration/deceleration
time
80
constant of MPG
Setting range：0～400 （ms）
0154
The acceleration clamping time constant of MPG
100
Setting range：0～400 （ms）
383
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0155
The top clamping speed of single feed
Setting range：0～3000
0156
1000
（mm/min）
The linear acceleration/deceleration time constant of
100
JOG feed along each axis
Setting range：0～400 （ms）
0157
The
exponential
acceleration/deceleration
time
120
MPG
50
The 1st axis command frequency-multiplication
1
constant of JOG feed along each axis
Setting range：0～400 （ms）
0158
The
acceleration
clamping
constant
of
incomplete operation mode
Setting range：0～1000 （ms）
0160
coefficient (CMR)
Setting range：1～65536
APPEDIX
0161
The 2nd axis command frequency-multiplication
1
coefficient (CMR)
Setting range：1～65536
0162
The 3rd axis command frequency-multiplication
1
coefficient (CMR)
Setting range：1～65536
0163
The 4th axis command frequency-multiplication
1
coefficient (CMR)
Setting range：1～65536
0164
The 5th axis command frequency-multiplication
coefficient (CMR)
Setting range：1～65536
384
1
Appendix One GSK218MC Parameter List
0165
The 1st axis command frequency-division coefficient
1
(CMD)
Setting range：1～65536
0166
The 2nd axis command frequency-division coefficient
1
(CMD)
Setting range：1～65536
0167
The 3rd axis command frequency-division coefficient
1
(CMD)
Setting range：1～65536
0168
The 4th axis command frequency-division coefficient
1
(CMD)
Setting range：1～65536
0169
The 5th axis command frequency-division coefficient
1
(CMD)
Setting range：1～65536
The 1st axis
manual position at the rapid traverse
5000
manual position at the rapid traverse
5000
manual position at the rapid traverse
5000
manual position at the rapid traverse
5000
APPEDIX
0170
rate
Setting range：0～30000
0171
The 2nd axis
rate
Setting range：0～30000
0172
The 3rd axis
rate
Setting range：0～30000
0173
The 4th axis
rate
Setting range：0～30000
385
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0174
The 5th axis
manual position at the rapid traverse
5000
rate
Setting range：0～30000
0175
The program name of the 1st axis
Setting range：0～8
0176
0177
0179
0180
3
(0:X 1:Y 2:Z 3:A 4:B 5:C 6:U 7:V 8:W)
The program name of the 5th axis
Setting range：0～8
2
(0:X 1:Y 2:Z 3:A 4:B 5:C 6:U 7:V 8:W)
The program name of the 4th axis
Setting range：0～8
1
(0:X 1:Y 2:Z 3:A 4:B 5:C 6:U 7:V 8:W)
The program name of the 3rd axis
Setting range：0～8
0178
(0:X 1:Y 2:Z 3:A 4:B 5:C 6:U 7:V 8:W)
The program name of the 2nd axis
Setting range：0～8
0
4
(0:X 1:Y 2:Z 3:A 4:B 5:C 6:U 7:V 8:W)
The grid or reference position offset value of the 1st
0
APPEDIX
axis
Setting range：0～50
0181
The grid or reference position offset value of the 2nd
0
axis
Setting range：0～50
0182
The grid or reference position offset value of the 3rd
0
axis
Setting range：0～50
0183
The grid or reference position offset value of the 4th
0
axis
Setting range：0～50
0184
386
The compensation condition when the friction
1
Appendix One GSK218MC Parameter List
compensation along Z axis of the machine tool is
performed (Default: 1.0)
Setting range：0～50
0185
The friction compensation method along Z axis of
1
machine tool
Setting range：0～50
0: Disabled, 1: Up, 2: Down, 3: Up or Down
0186
The friction compensation value along Z axis of
0.5
machine tool (mm)
Setting range：0～0.5
0187
Reverse interval compensation condition along Z
1
axis (Default: 1)
Setting range：0～50
0188
Reverse
interval
compensation
accumulation
0.02
distance along Z axis (Default: 0.02)
Setting range：0～0.5
Reverse interval compensation condition along Z
APPEDIX
0189
0.0100
axis (Default: 1)
Setting range：0.0001～1.0000 (mm)
Set
α = p(189) × 0.0001 , after the feed is reversed; single servo period feed value is more than α ,
and the reverse interval compensation begins.
Ttherefore, when the excircle outline with bigger radius is machined, the least accuracy should be set
for guard against that the compensation position does not deviate position of the pass-quadrant. In
the machining curve surface, to avoid each tool path is performed the reverse interval compensation
at a fixed position, so that a raised ridge occurs, and therefore, the bigger accuracy should be set to
evenly distribute the interval compensation within a specified width.
0190
The reverse interval compensation value of the 1st
0.0000
axis
Setting range：
Metric: -0.5～0.5 (mm)
387
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Inch: -0.5～0.5/25.4 (inch)
Rotation axis: -0.5～0.5000 (deg)
0191
The reverse interval compensation value of the 2nd
0.0000
axis
Setting range：
Metric: -0.5～0.5 (mm)
Inch: -0.5～0.5/25.4 (inch)
Rotation axis: -0.5～0.5 (deg)
0192
The reverse interval compensation value of the 3rd
0.0000
axis
Setting range：
Metric: -0.5～0.5 (mm)
Inch: -0.5～0.5/25.4 (inch)
Rotation axis: -0.5～0.5 (deg)
0193
The reverse interval compensation value of the 4th
0.0000
axis
Setting range：
APPEDIX
Metric: -0.5～0.5 (mm)
Inch: -0.5～0.5/25.4(inch)
Rotation axis: -0.5～0.5(deg)
0194
The reverse interval compensation value of the 5th
0.0000
axis
Setting range：
Metric: -0.5～0.5(mm)
Inch: -0.5～0.5/25.4(inch)
Rotation axis: -0.5～0.5 (deg)
0195
The compensation step length of the 1st axis interval
based upon the fixed frequency compensation
method
Setting range：0～0.5
388
(mm)
0.0030
Appendix One GSK218MC Parameter List
0196
The compensation step length of the 2nd axis interval
0.0030
based upon the fixed frequency compensation
method
Setting range：0～0.5
0197
(mm)
The compensation step length of the 3rd axis interval
0.0030
based upon the fixed frequency compensation
method
Setting range：0～0.5
0198
(mm)
The compensation step length of the 4th axis interval
0.0030
based upon the fixed frequency compensation
method
Setting range：0～0.5
0199
(mm)
The compensation step length of the 5th axis interval
0.0030
based upon the fixed frequency compensation
method
Setting range：0～0.5
The time constant of the reverse interval based upon
20
APPEDIX
0200
(mm)
the speed up/down compensation method
Setting range：0～400 （ms）
0201
Reverse interval compensation method
0
Setting range：0～2
0: Modal A, 1: Modal B,
0202
2: Modal C
The acceptance width of completion signal of the M,
0
S and T signals.
Setting range：0～9999 （ms）
0203
Output time of resetting signal
200
Setting range：50～400 (ms)
0204
The allowable digit of M code
2
Setting range：1～2
389
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0205
The allowable digit of S code
5
Setting range：1～6
0206
The allowable digit of T code
4
Setting range：1～4
0210
The incremental value of the number when the
10
sequence number is automatically inserted.
Setting range：0～1000
0211
Prohibt the beginning number of the tool offset value
0
inputted by MDI
Setting range：0～9999
0212
Prohibt the number of the tool offset value inputted
0
by MDI
Setting range：0～9999
0214
The limit value of circular arc radius error
0.05
APPEDIX
Setting range：0.0001～0.1000 （mm）
0216
Pitch error compensation number of the 1st axis
0
reference position
Setting range：0～9999
0217
Pitch error compensation number of the 2nd axis
0
reference position
Setting range：0～9999
0218
Pitch error compensation number of the 3rd axis
0
reference position
Setting range：0～9999
0219
Pitch error compensation number of the 4th axis
reference position
390
0
Appendix One GSK218MC Parameter List
Setting range：0～9999
0220
Pitch error compensation number of the 5th axis
0
reference position
Setting range：0～9999
0226
The pitch error compensation interval of the 1st axis
5
Setting range：0～9999.9999
0227
The pitch error compensation interval of the 2nd axis
5
Setting range：0～9999.9999
0228
The pitch error compensation interval of the 3rd axis
5
Setting range：0～9999.9999
0229
The pitch error compensation interval of the 4th axis
5
Setting range：0～9999.9999
0230
The pitch error compensation interval of the 5th axis
5
Setting range：0～9999.9999
The reverse interval compensation value of the 1st
APPEDIX
0231
0
axis at the rapid traverse rate
Setting range：-0.5～0.5
0232
The reverse interval compensation value of the 2nd
0
axis at the rapid traverse rate
Setting range：-0.5～0.5
0233
The reverse interval compensation value of the 3rd
0
axis at the rapid traverse rate
Setting range：-0.5～0.5
0234
The reverse interval compensation value of the 4th
0
axis at the rapid traverse rate
Setting range：-0.5～0.5
391
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0235
The reverse interval compensation value of the 5th
0
axis at the rapid traverse rate
Setting range：-0.5～0.5
0236
Circular arc pointed angle disposes parameter 1
0
Setting range：0～5
0237
Circular arc pointed angle disposes parameter 2
0
Setting range：0～5
0238
Circular arc pointed angle disposes parameter 3
0
Setting range：0～5
0240
The gain adjustment data of the spindle speed
1
analog output
Setting range：0.98～1.02
0241
The compensation value of the offset voltage for the
0
spindle speed analog output
APPEDIX
Setting range：-0.2～0.2
0242
The spindle speed in the spindle orientation or JOG
50
Setting range：0～9999 (r/min)
0243
The Max. setting value of the frequency-converter
8191
Setting range：4000～8191
0246
The spindle Max. speed corresponding to the gear 1
6000
Setting range：0～99999 (r/min)
0247
The spindle Max. speed corresponding to the gear 2
6000
Setting range：0～99999 (r/min)
0248
The spindle Max. speed corresponding to the gear 3
Setting range：0～99999 (r/min)
392
6000
Appendix One GSK218MC Parameter List
0250
The motor speed in the spindle gear shifting
Setting range：0～1000
0251
50
(r/min)
The top motor speed in the spindle gear shifting
6000
Setting range：0～99999 (r/min)
0254
The axis regards as the count reference in the
0
surface speed control
Setting range：0～4
0255
The lowest speed in the constant surface speed
100
control (G96)
Setting range：0～9999
0257
(r/min)
Spindle upper-limit speed in tapping cycle
2000
Setting range：0～5000 (r/min)
0258
Spindle upper-limit speed
6000
Setting range：0～99999 (r/min)
Spindle encoder linear number
APPEDIX
0261
1024
Setting range：0～9999
0262
Spindle override lower-limit value
0.5000
Setting range：0.5～1
0266
The limit value is ignored moving along the external side
0
of the corner in the cutter compensation C
Setting range：0～9999.9999
0267
The top value of the cutter wear compensation value
Setting range：0～999.9999
0268
400.0000
(mm)
The Max. error value of the cutter compensation C
0.0010
Setting range：0.0001~0.0100
393
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0269
The cutter radius coefficient with helix in groove
1.5000
cycle
Setting range：0.0100～3.0000
0270
The clearance of G73 in high-speed peck cycle
Setting range：0～999.9999
0271
0281
(mm)
The clearance value of G83 in canned cycle
Setting range：0～999.9999
2.0000
2.0000
(mm)
The least dwell time at the bottom of a hole
250
Setting range：0～1000 (ms)
0282
The top dwell time at the bottom of a hole
9999
Setting range：1000～9999 (ms)
0283
The override value in the rigid tapping tool-retraction
100
Setting range：0～100
Note: When the override value of the bit 4 of parameter N.:44 =1 is enabled.
APPEDIX
When the bit of parameter No.: 45 equals to 1, the data unit to be set is regarded as 10%, up to
1000% override value can be set.
0284
The retraction value or clearance value in the peck
0
tapping cycle
Setting range：0～100 (mm)
0286
The gear’s number at the side of the spindle (the 1st
1
gear)
Setting range：1～999
0287
The gear’s number at the side of the spindle (the 2nd
1
gear)
Setting range：1～999
0288
394
The gear’s number at the side of the spindle (the 3rd
1
Appendix One GSK218MC Parameter List
gear)
Setting range：1～999
0290
The gear’s number at the side of the position
1
st
encoder side (the 1 gear)
Setting range：1～999
0291
The gear’s number at the side of the position
1
encoder side (the 2nd gear)
Setting range：1～999
0292
The gear’s number at the side of the position
1
rd
encoder side (the 3 gear)
Setting range：1～999
0294
The top speed of the spindle in rigid tapping (the 1st
6000
gear)
Setting range：0～9999 (r/min)
0295
The top speed of the spindle in rigid tapping (the 2nd
6000
APPEDIX
gear)
Setting range：0～9999 (r/min)
0296
The top speed of the spindle in rigid tapping (the 3rd
6000
gear)
Setting range：0～9999
0298
(r/min)
The linear acceleration/deceleration time constant of
200
st
the spindle and tapping axis (the 1 gear)
Setting range：0～9999 （ms）
0299
The linear acceleration/deceleration time constant of
nd
the spindle and tapping axis (the 2
200
gear)
Setting range：0～9999 （ms）
0300
The linear acceleration/deceleration time constant of
200
395
GSK218MC Series Machining Center CNC System Programming & Operation Manual
the spindle and tapping axis (the 3rd gear)
Setting range：0～9999 （ms）
0302
The time constant both the spindle and tapping axis
200
st
in tool-retraction (the 1 gear)
Setting range：0～9999 （ms）
0303
The time constant both the spindle and tapping axis
200
in tool-retraction (the 2nd gear)
Setting range：0～9999 （ms）
0304
The time constant both the spindle and tapping axis
200
rd
in tool-retraction (the 3 gear)
Setting range：0～9999 （ms）
0310
It is regarded as the speed allowance rate (q) when
5
the spindle reaches to the command speed
Setting range： 0～1000
0311
Spindle fluctuation rate (r) without issuing the
5
APPEDIX
detection alarm of the spindle speed alteration
Setting range： 0～1000
0312
Fluctuation amplitude (i) of the spindle speed without
10
the detection alarm of spindle speed alternation
Setting range： 0～9999
0313
Spindle speed fluctuation detection time (p)ms from
1000
the command speed change to the beginning.
Setting range： 0～99999
0320
The clearance value of spindle in rigid tapping (the
0
st
1 gear)
Setting range：0～99.9999
0321
396
The clearance value of spindle in rigid tapping (the
0
Appendix One GSK218MC Parameter List
2nd gear)
Setting range：0～99.9999
0322
The clearance value of spindle in rigid tapping (the
0
rd
3 gear)
Setting range：0～99.9999
0323
Spindle command multiplication coefficient (CMR)
512
(the 1st gear)
Setting range：0～9999
0324
Spindle command multiplication coefficient (CMR)
nd
(the 2
512
gear)
Setting range：0～9999
0325
Spindle command multiplication coefficient (CMR)
512
(the 3rd gear)
Setting range：0～9999
0326
Spindle
command
frequency-division
coefficient
125
frequency-division
coefficient
125
frequency-division
coefficient
125
st
APPEDIX
(CMD) (the 1 gear)
Setting range：0～9999
0327
Spindle
command
(CMD) (the 2
nd
gear)
Setting range：0～9999
0328
Spindle
command
rd
(CMD) (the 3 gear)
Setting range：0～9999
0329
The used rotation angle in the coordinate rotation
0
when the rotation angle command does not perform.
Setting range：0～9999.9999
0330
The used scaling override when using without the
1
397
GSK218MC Series Machining Center CNC System Programming & Operation Manual
scaling override command
Setting range：0.0001～9999.9999
0331
The 1st axis scaling override
1
Setting range：0.0001～9999.9999
0332
The 2nd axis scaling override
1
Setting range：0.0001～9999.9999
0333
The 3rd axis scaling override
1
Setting range：0.0001～9999.9999
0334
The dwell time in the unidirection orientation
0
Setting range：0～10(S)
0335
The unidirection orientation and overtravel value
0
st
along the 1 axis
Setting range：-99.9999～99.9999
APPEDIX
0336
The unidirection orientation and overtravel value
nd
along the 2
0
axis
Setting range：-99.9999～99.9999
0337
The unidirection orientation and overtravel value
0
along the 3rd axis
Setting range：-99.9999～99.9999
0338
The unidirection orientation and overtravel value
0
th
along the 4 axis
Setting range：-99.9999～99.9999
0339
The unidirection orientation and overtravel value
along the 5th axis
Setting range：-99.9999～99.9999
398
0
Appendix One GSK218MC Parameter List
0341
The buffering area dimension of ARM interpolation
36
point
Setting range：0～99999
0342
The low speed of the 1st axis zero return
200
Setting range：0～1000
0343
The low speed of the 2nd axis zero return
200
Setting range：0～1000
0344
The low speed of the 3rd axis zero return
200
Setting range：0～1000
0345
The low speed of the 4th axis zero return
200
Setting range：0～1000
0346
The low speed of the 5th axis zero return
200
Setting range：0～1000
0347
The absolute position of the 1st axis reference
65000
APPEDIX
position when using the absolute rotation encoder.
Setting range：0～131071
0348
The absolute position of the 2nd axis reference
65000
position when using the absolute rotation encoder.
Setting range：0～131071
0349
The absolute position of the 3rd axis reference
65000
position when using the absolute rotation encoder.
Setting range：0～131071
0350
The absolute position of the 4th axis reference
65000
position when using the absolute rotation encoder.
Setting range：0～131071
0351
The absolute position of the 5th axis reference
65000
399
GSK218MC Series Machining Center CNC System Programming & Operation Manual
position when using the absolute rotation encoder.
Setting range：0～131071
0352
Acceleration/deceleration
time
constant
with
60
time
constant
with
100
high-speed in zero return
Setting range：3～400
0353
Acceleration/deceleration
low-speed in zero return
Setting range：3～400
0354
Failure times of DSP start
0
Setting range：0～999999
0355
Successful times of system start
0
Setting range：0～999999
0356
The machined components
0
Setting range：0～9999
APPEDIX
0357
The total components to be machined
0
Setting range：0～9999
0358
The accumulation value (Hours) of power-on time
0
Setting range：0～99999
0359
The accumulation value (Days) of power-on time
0
Setting range：0～99999
0360
The accumulation value of cutting time (Hours)
0
Setting range：0～99999
0361
Backup the connection state (Unchangeable) without
MDT package of the Ethernet
Setting range：0～20
400
0
Appendix One GSK218MC Parameter List
0362
Backup DSP scan counter (Unchangeable)
78
Setting range：0～1000
0363
Backup
the
invalid
MDT
package
counter
0
Backup the consecutive times (Unchangeable)
0
(Unchangeable) of the Ethernet
Setting range：0～99999
0364
without MDT package of the Ehternet
Setting range：0～99999
0365
Backup the connection state (Unchangeable) without
0
MDT package of the Ehternet
Setting range：0～99999
0371
The reverse position tolerance along the 1st axis
0.0150
Setting range：0～99.9999 (mm)
0372
The reverse position tolerance along the 2nd axis
0.0150
Setting range：0～99.9999 (mm)
The reverse position tolerance along the 3rd axis
APPEDIX
0373
0.0150
Setting range：0～99.9999 (mm)
0374
The reverse position tolerance along the 4th axis
0.0150
Setting range：0～99.9999 (mm)
0375
The reverse position tolerance along the 5th axis
0.0150
Setting range：0～99.9999 (mm)
When the reverse interval compensation values (P0190---P0193) set by one axis is more than the
inversion position tolerances (P0371---P0374)set by this axis, one single-unit end speed before the
reverse interval compensation beginning of this axis reduces to the lowest speed, so that the other
axes within the interval compensation period moves a lesser position to ensure that the compound
path is lesser deviated from the true path.
401
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0376
Each axis sequence moves to the program restart
12345
position
Setting range：0～99999
0380
Set the synchronized axis with the 4th one 0: no
synchronization with any axis
nd
2
axis
1: the 1st axis
0
2: the
rd
3: the 3 axis
Setting range：0～3
0381
The top allowable error among the synchronization
200
axes
Setting range：0～10000
0382
Set the D-value of dual-drive reference position
0.0000
Setting range：0.0000～2000.0000
0387
The position value of tool-setter in G53 along the 1st
0
axis
Setting range：-999.9999～999.9999
APPEDIX
0388
The position value of tool-setter in G53 along the 2nd
0
axis
Setting range：-999.9999～999.9999
0389
The position value of tool-setter in G53 along the 3rd
0
axis
Setting range：-999.9999～999.9999
0390
The estimated length from the current tool point to the
0
fixture
Setting range： 0.0000～999.9999
0391
The diameter of automatic prober
2
Setting range： 0.5000～999.9999
0392
402
The movement distance of the servo optimization
50
Appendix One GSK218MC Parameter List
Setting range： 0～100
0393
The movement rate of the servo optimization
2000
Setting range： 0～5000
0394
Coordinate system back up along 1st axis
0
Setting range： -9999.9999～9999.9999
0395
Coordinate system back up along 2nd axis
0
Setting range： -9999.9999～9999.9999
0396
Coordinate system back up along 3rd axis
0
Setting range： -9999.9999～9999.9999
0397
Coordinate system back up along 4th axis
0
Setting range： -9999.9999～9999.9999
0398
Coordinate system back up along 5th axis
0
Setting range： -9999.9999～9999.9999
Interpolation step-length times
APPEDIX
0399
1.5
Setting range： 1.0000～10.0000
0400
Shape matched parameter
20
Setting range：0.0020～99.0000
The shap matched parameter (#400) is performed the shape optimization based upon the initial
spline and the analysis shape error, and control the error within the allowable range.
The greater the parameter is, the greater the shape error is. The smaller the parameter is, the smaller
the shape error is.
0401
Shape matched limit
15
Setting range：1.0000～999.000
The shape matched limit parameter (#401) can be restricted error fluctuation on shape due to the
curvature optimization when the speed mating calculation is performed.
0402
Speed matched parameter
1
403
GSK218MC Series Machining Center CNC System Programming & Operation Manual
Setting range：0.0020～99.0000
Speed matched parameter (#402) is the curvature on curve which shows the radial-shape along the
normals of each point on the curve to optimize the curvature and smooth the speed.
The bigger the parameter is, the lower the curvature optimization is, and the greater the machining
speed is, the shorter the machining time is.
The smaller the parameter is, the higher the curvature optimization is, the longer the machining time
is.
0403
The fitting section number of small-line-block
7
Setting range：0.0020～999.0000
This parameter (#403) determines the cutter position points of the fitting spline curve, which should
be controlled within a certain range.
#403 = 1~10
the greater the parameter is, the more the calculation value is, the less the shape error
is.
the smaller the parameter is, the smaller the calculation value is, the greater the shape
error is.
0404
Spline coefficient n1
30
Setting range：1.0000～199.0000
APPEDIX
0405
Spline coefficient n2
30
Setting range：1.0000～199.0000
0406
Spline coefficient n3
30
Setting range：1.0000～199.0000
Fit a piece of initial spline curves for 3 times based upon the spline coefficients n1,n2,n3 (#404, #405,
#406); the greater the spline coefficients are, the greater the curve errors are, however the speed is
smooth and the machine operates stably. The least the coefficients are, the least the curve errors are,
but the speed does not smooth and the machine viberates. The spline coefficient n3 (#406) is
reversed.
0407
System internal parameter 1
Setting range：0.0020～99.0000
404
0.6000
Appendix One GSK218MC Parameter List
0408
System internal parameter 2
0.6000
Setting range：0.0020～99.0000
0409
Pre-read the smooth treatment control
2.0000
Setting range：0.0000～30.0000
The parameter of the pre-reading treatment control is pre-read the machining shape in advance,
automatically calculate the tendency of the integral shape, so reduce machining scars due to the
program error generated from the CAM.
0: Close the pre-reading smooth treatment function
1: Perform the smooth treatment based upon the length
2: Perform the smooth treatment based upon the integrated relationships between length and angle
0410
Accuracy smooth balance coefficient
10.0000
Setting range：0.0000～10.0000
If you want to carry out the high-accuracy control, the setting value can only be set for the
parameter accuracy smooth balance coefficient (#410), this parameter can be controlled the
machining level. Total 11 levels (0-10);
#410 = 0: High accuracy control, strictly control the in-position accuracy, regardless of the
smooth, it is enable to program for machining the meticulous edge type (for example: word).
is; the higher the lever is, the better the smooth is.
Adjust this parameter to reach an ideal effect.
0411
Spline shape control coefficient
10.0000
Setting range：0.0000～10.0000
0412
Fitting accuracy control for small-line-block
-1.0000
Setting range：-10.0000～50.0000
0413
Roundness smooth control coefficient n1
3.0000
Setting range：0.0000～50.0000
0414
Roundness smooth control coefficient n2
0.0000
Setting range：0.0000～50.0000
405
APPEDIX
=1-10: Return to the high-speed accuracy contro. The lower the level is, the better the accuracy
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0444
The Max. allowable error between the machine
50
coordinate and absolute encoder position of each
axis
Setting range：0～500
0445
Axis 1 configures griding accuracy
0.0010
Setting range：0～10
0446
Axis 2 configures griding accuracy
0.0010
Setting range：0～10
0447
Axis 3 configures griding accuracy
0.0010
Setting range：0～10
0448
Axis 4 configures griding accuracy
0.0010
Setting range：0～10
0449
Axis 5 configures griding accuracy
0.0010
Setting range：0～10
APPEDIX
0450
Machine stroke detection: the absolute position of
st
the 1
0.0000
axis encoder along negative direction
boundary
Setting range：-99999.999～99999.999
0451
Machine stroke detection: the absolute position of
st
the 1
0.0000
axis encoder along positive direction
boundary
Setting range：-99999.999～99999.999
0452
Machine stroke detection: the absolute position of
nd
the 2
0.0000
axis encoder along negative direction
boundary
Setting range：-99999.999～99999.999
0453
406
Machine stroke detection: the absolute position of
0.0000
Appendix One GSK218MC Parameter List
the 2nd axis encoder along positive direction
boundary
Setting range：-99999.999～99999.999
0454
Machine stroke detection: the absolute position of
0.0000
the 3rd axis encoder along negative direction
boundary
Setting range：-99999.999～99999.999
0455
Machine stroke detection: the absolute position of
0.0000
the 3rd axis encoder along positive direction
boundary
Setting range：-99999.999～99999.999
0456
Machine stroke detection: the absolute position of
0.0000
the 4th axis encoder along negative direction
boundary
Setting range：-99999.999～99999.999
0457
Machine stroke detection: the absolute position of
0.0000
APPEDIX
the 4th axis encoder along positive direction
boundary
Setting range：-99999.999～99999.999
0458
Machine stroke detection: the absolute position of
0.0000
the 5th axis encoder along negative direction
boundary
Setting range：-99999.999～99999.999
0459
Machine stroke detection: the absolute position of
0.0000
the 5th axis encoder along positive direction
boundary
Setting range：-99999.999～99999.999
407
GSK218MC Series Machining Center CNC System Programming & Operation Manual
APPEDIX
408
Appendix Two
Alarm List
Appendix Two
Content
No.
0000
The parameter must to be cut the power once that is altered.
0001
Fail to open the file
0002
The MDI data exceeds its range.
0003
The copied or renamed program No. exists.
0004
0005
0006
0007
A number or the sign “_” was input without an address at the beginning of a
block. Modify the program
The address was not followed by the appropriate data but was followed by
another address or EOB code. Modify the program.
Sign “-“ input error (Sign “-“ was input followed with an address which it can
not be used the “-“ or two or more “-“ signs were input). Modify the program
Sign “.“ input error (Sign “.“ was input in an address which it can not be used
the “.“ or two or more “.“ signs were input). Modify the program
0008
Program file excessive big. It is better to transfer by DNC.
0009
Illegal address input. Modify the program
0011
0012
0013
An unusable G code is used or a G code without this function is commanded.
Modify the program.
Feedrate was not commanded to a cutting feed or the feedrate was
inadequate. Modify the program.
Inadequate disc space. Fail to create a new file or add file content.
Fail to create a new program due to the program file numbers are reached to
the upper-limit.
0014
It can not specify the G95, without supporting from spindle
0015
The allowed simultaneously controlled axes are exceeded.
0016
The current pitch error compensation exceeds its range.
0017
0018
0019
0020
APPEDIX
0010
Remark
Alarm
Alarm List
Inadequate authority modification, input the corresponding password to the
password interface.
Do not modify the null and local variable. G10 is only altered the parameter
for the user level.
Without scaling function, if you want to use it, it is better to open it by altering
the bit parameter 60.5.
In circular interpolation (G02 or G03), the distance between start and arc
409
GSK218MC Series Machining Center CNC System Programming & Operation Manual
center is different from the one between the end and arc center, the D-value
exceeds the value specified in the data parameter 214.
0021
0022
0023
0024
0025
0026
0027
0028
0029
An axis not included in the selected plane (by using G17,G18,G19) was
commanded in circular interpolation. Modify the program.
In the circular interpolation, neither R (Specifying an arc radius) nor I, J and K
(Specifying the distance from a start point to the center) is specified.
In the arc interpolation, I, J, K and R are simultaneously specified.
Helical interpolation, helical angle is set to 0; the system does not be treated.
Modify the program.
G12 can not be shared a same block with G command.
The file format of which the system does not support. The file is enormous or
the line length of the file exceeds 1024 bytes.
Length cutter compensation command can not be shared a same block with
G92. Modify the program.
In the plane selection command, two or more axes on the same diretion are
commanded. Modify the program.
The compensation value specified by D/H code is excessive large. Modify
the program
The tool length compensation number or the cutter compensation number
0030
specified by D/H is excessive large. Additionally, the workpiece coordinate
system number specified by P code is also too large. Modify the program
APPEDIX
When G10 sets the offset amount, workpiece coordinate system, external
0031
workpiece coordinate system and additional workpiece coordinate system,
the specified P value is excessive big or does not be specified.
In setting an offset amount by G10 or in writing an offset amount by system
0032
variables, the offset amount was excessive or does not be specified. Modify
the program.
0033
0034
0036
0037
0038
0039
410
A intersection point can not be determined in a cutter compensation C or a
chamfering. Modify the program.
The cutter compensation can not be set up or cancelled in the arc command.
Modify the program.
Skip cutting (G31) was specified in cutter compensation mode. Modify the
program.
The plane selected by using the G17, G18 or G19 is changed in cutter
compensation C mode. Modify the program
Overcutting will occur in cutter compensation C because the arc start point or
end coincides with the arc center. Modify the program.
The cutter nose positioning in the cutter compensation C is incorrect.
Appendix Two
Alarm List
The workpiece coordinate system can not be converted in cutter
0040
compensation C. The coordinate system conversion can only be performed
after the cutter compensation is cancelled.
0041
Overcutting will occur and interference generates in cutter compensation C.
Modify the program.
In the cutter compensation, more than 10 blocks without movement
0042
command but the dwell command are consecutively performed. Modify the
program.
0043
0044
0045
0046
0047
The authority can be changed at the password interface if the authority is
absent.
One of G27, G28, G29 or G30 is commanded in canned cycle mode. Modify
the program
In the canned cycle G73/G83, a depth for each cutting (Q) is not specified or
Q value is regarded as 0. Modify the program.
The commands other than P2, P3 and P4 are specified in the 2nd, 3rd and 4th
reference position return command.
Firstly perform the machine zero before executing the commands such as
the G28, G30 and G53, etc.
0048
In the canned cycle, Z plane should be higher than the R plane.
0049
In the canned cycle, Z plane should be lower than the R plane.
0050
The position should be moved when changing the canned cycle method.
0051
APPEDIX
Improper movement operation or move distance is specified in block followed
with the chamfering round angle or chamfering oblique angle. Modify the
program.
0052
0053
The canned cycle in milling groove can not be used the image function.
Modify the program.
Incorrect chamfering oblique angle or chamfering round angle command
format. Modify the program.
0054
DNC transmission error
0055
Fail to complete the chamfering movement
0056
0057
0058
M99 can not be shared a same block with the macro program command
(G65). Modify the program.
Fail to write the file. It is necessary to restart after the power is turned off.
In an arbitrary chamfering oblique angle or chamfering round angle block, a
specified axis is not within the selected plane. Modify the program.
In an external program number search, a specified program number was not
0059
found or a specified program is being edited in background. Check the
program number and external signal. Or discontinue the background editing.
411
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0060
A specified sequence number was not found in the sequence number search.
Check the sequence number.
0061
The 1st axis is out of the reference position
0062
The 2nd axis is out of the reference position
0063
The 3rd axis is out of the reference position
0064
The 4th axis is out of the reference position
0065
The 5th axis is out of the reference position
0066
It is necessary to cancel the canned cycle mode before performing the
parameter input (G10).
0067
The setting format does not be supported by G10.
0068
Fail to open the parameter switch
0069
The U-disc operation interface should be closed when machining.
0070
The memory area is insufficient. Delete any unnecessary program, then retry.
0071
0072
0073
The address to be searched was not found. Or the program with specified
program number was not found in program index. Check the data.
The stored program numbers are exceeded 400. Delete unnecessary
programs.
The program number being specified is used. Change the program number
or delete the unnecessary programs.
0074
The program number is other than 1 to 99999. Change the program number.
0075
An attempt was made to register a program whose number was protected.
APPEDIX
0076
0077
0078
0079
0080
Address P (Program number) was not commanded in the block which
includes an M98. Modify the program.
The program was called in five folds. Modify the program.
The program number specified by address P in the block which includes G98
and G65 was not found or the macro program called by M06 does not exist.
The system is expired, contact the supplier.
Unreasonable MDI data, the Max. speed is less than the Min. speed; or the
lowest speed is more than the top speed.
0081
Macro program cannot be called the subprogram. Modify the program.
0084
Button overtime or short-circuit occurs.
0085
0086
When the data is input to memory by using the series port, overflow occurs.
The setting or input/output equipment of Baud rate is incorrect.
In the canned cycle modal, the system cannot be shifted the panel.
Alarm No. 0087~0091 are the start points of the reference position return
0087
along each axis of which the reference position return can not be performed
due to the alarm numbers are too close to the reference position or it is so
slowly. The reference position should be departed from the start as far as
412
Appendix Two
Alarm List
possible. Alternatively, the reference position should be specified the fast rate
for the reference position return.
0092
G27 command can not return to the reference position.
0093
Unmatch motor type
0098
0100
A program restart is performed without the reference position return after
Power ON or ESP, and G28 was found in program.
On the PARAMETER (SETTING) screen, PWE (parameter writing enabled)
is set to 1. Set it to 0, then reset the system.
0101
Power-off memory data disorder, ensure that the position is correct.
0102
The motor type parameter between the system and drive are inconsistent.
0103
Bus communication error. Check the reliability of the reticle.
0104
Machine tool zero setting overtime
0105
Drive data gain overtime
0106
The drive is inconsistent with the gear ratio of the system servo parameter.
0107
The parameters between the drive and system servo are inconsistent.
0108
Insert the U disk
0110
The position data exceeds the allowance range. Perform the zero return.
0111
0112
0113
1047 ).
Division by zero was specified (including tan90°)
A function command which cannot be used in custom macro is specified.
Modify the program.
APPEDIX
0114
The calculation is out of the allowable range (-1047 to -10-29, 0 and 10-29 to
G39 format error. Modify the program.
The value regarded as the variable can not be specified. Alternatively, the O,
0115
N regarded as variable are specified in the user marco program. Modify the
program.
0116
0117
0118
0119
The left side of assignment statement is a variable whose an assignment is
inhibited. Modify the program.
This parameter does not support the G10 on-line modification. Alter the
program.
The nesting of bracket exceeds the upper limit (quintuple). Modify the
program.
M00,M01,M02,M30,M98,M99,M06 commandes can not be shared with a
same block with other M codes.
0120
Partion setting is being recovered.
0121
The machine tool coordinate and the encoder feedback value are exceed the
setting value of the offset.
0122
The nesting layers of the marco program calling are more than 5. modify the
413
GSK218MC Series Machining Center CNC System Programming & Operation Manual
program.
0123
0124
The transmission and cycle statement can not be used in the MDI current
modal and DNC mode.
Program illegal end, without M30 or M02 or M99 command, or without the
end symbol. Modify the program.
0125
Format error in macro. Modify the program.
0126
Program cycle failed. Modify the program.
0127
0128
0129
NC and user macro command statement are existed together. Modify the
program.
The sequence number specified in the branch command was not 0-99999.
Or, it cannot be found. Modify the program.
An address of <Argument assignment> is incorrect. Modify the program.
An axis control command was given by PLC to an axis controlled by CNC. Or
0130
an axis control command was given by CNC to an axis controlled by PLC.
Modify the program.
0131
Five or more alarms have generated in external alarm message. Check the
ladder diagram.
0132
No alarm in external alarm message. Check the PLC.
0133
The axis command does not be supported by system. Modify the program.
0135
APPEDIX
0136
0137
0138
The index angle of the index worktable does not the multiple of the angle unit.
Modify the program.
In the index worktable, another axis was instructed with the B axis together.
Modify the program.
Skip the sequence number to be transferred by command within the cycle.
Modify the program.
Cycle statement dismatches or skip command enters into the cycle. Modify
the program.
0139
PLC axis control selection error. Modify the program
0140
The sequence number of the macro command skip is absent.
0141
MDI current modal and DNC mode does not support the macro command
skip.
The proportion scaling override other than from 1 to 999999 is specified.
0142
Scaling magnification is specified in other than 1 – 999999. Correct the
scaling setting.
The scaling results, move distance, coordinate value and circular radius
0143
exceed the Max. command value. Correct the program or scaling
magnification.
0144
414
The coordinate rotation plane should be idencial with the arc or cutter
Appendix Two
Alarm List
compensation C plane. Modify the program.
0145
0148
0160
0161
0163
0164
0165
G28 command is already specified when the reference position does not
establish yet. Modify the program or alter the bit 3 of parameter No.4 (AZR).
Automatic corner deceleration rate is out of the settable value of judgement
angle. Modify the parameter.
Acr can only be used by R programming in the polar coordinate mode.
In the polar coordinate mode, the relevant commands, such as the reference
point, plane selection or direction can not be performed.
In the rotation mode, the relevant G commands, such as the reference point
or coordinate system can not be performed.
In the scaling mode, the relevant G commands such as the reference point or
coordinate system can not be performed.
It is better to speicify the rotation, scaling or G10 command with a single
block.
0166
There is no specification axis when reference point return.
0167
Intermediate point coordinate excessive big
0168
0170
0172
The Min. dwell time at the bottom of a hole should be less than the Max. one
at the bottom of a hole.
Cutter compensation does not cancel when entering or retracting eh
subprogram.
P does not the integer, alternatively, P is less than or equals to 0 in the block
0173
The subprogram calling should be less than 9999 times.
0175
The canned cycle can only be performed on the G17 plane.
0176
The spindle speed does not specify before the rigid tapping begins.
0177
APPEDIX
for calling the subprogram.
The IO control below the G76 command does not support the orientation
function of the spindle. Modify the program or parameter.
0178
The spindle speed does not specify before the canned cycle begins.
0181
Illegal M codes
0182
Spindle speed excessive big or small
0183
Illegal T codes
0184
The selected tool is out of the range.
L is excessive small, the alarm reasons are shown below:
0185
1) L is less than the tool radius in the rectangle groove fine-milling.
2) L is less than 0 in the groove rough-milling.
L is excessive big, the alarm reasons are shown below:
0186
1) L is more than the cutter diameter in the circle groove rough-milling.
2) L is more than the cutter diameter in the rectangle groove rough-milling.
415
GSK218MC Series Machining Center CNC System Programming & Operation Manual
3) L is more than the I witin the rectangle groove in the finish-milling.
4) L is more than the J witin the rectangle groove in the finish-milling.
The cutter diameter is excessive big, the alarm reasons are shown below:
1) Cutter diameter is more than I in the interior circle groove rough-milling.
2) Cutter radius is more than the I-J in the interior circle groove fine-milling.
3) Cutter radius is more than J in the exterior circle groove fine-milling.
4) Cutter diameter is more than I within the rectangle groove in the
0187
fine/rough-milling.
5) Cutter diameter is more than J within the rectangle groove in the
fine/rough-milling.
6) Cutter radius is more than U within the rectangle groove in the
fine/rough-milling.
7) The cutter coefficient or the D is excessive big in helix. Modify the value of
the data parameter No.269 or the radius compensation value.
U is excessive big, the alarm reasons are shown below:
0188
1) Twice as much as U is more than I in the rectangle groove complex cycle.
2) Twice as much as U is more than J in the rectangle groove complex cycle.
APPEDIX
0189
U is excessive small, which should be more than or equals to cutter radius.
0190
V is excessive small or does not define, which should be more than 0.
0191
W is excessive small or does not define, which should be more than 0.
0192
Qis excessive small or does not define, which should be more than 0.
0193
I does not define or regards to 0.
0194
J does not define or regards to 0.
0195
D does not define or regards to 0.
In the constant surface cutting speed control, it is incorrect to specify an axis.
0198
(Refer to the parameter No.254). The command P of the specified axis is with
the illegal data. Modify the program.
0199
Undefined macro command. Modify the program.
In the rigid tap, an S value is out of the range or is not specified. The Max.
0200
value for S value can be specified by parameter. Change the setting in the
parameter or modify the program.
0201
In the rigid tapping, no F value is specified. Modify the program.
0202
In the rigid tapping, spindle distribution value is too large.
0203
0204
0205
416
In the rigid tapping, the position for a M code (M29) or a S command in
program is incorrect. Modify the program.
M29 should be specified in the G80 modal. Modify the program.
Rigid tapping signal is not 1 when G84 (or G74) is executed through the M
code (M29) is specified. Check the ladder diagram to find the reason.
Appendix Two
Alarm List
0206
Plane changeover was instructed in the rigid mode. Correct the program.
0207
The specified distance was too short or too long in rigid tapping.
0208
0209
0210
0212
0213
0214
0215
0216
0217
0218
0219
0221
0224
G10 modal firstly.
The scaling/rotation/polar coordinate modal does not support the program
restart.
The program restart file name is inconsistent. Select the correct file name.
Specify a chamfering or chamfering R, alternatively, there is an extral axis on
plane. Modify the program.
Tool-change marco program does not support the G31 skip. Modify the
program.
Tool-change macro program does support the skip operation.
Tool-change macro program does not support the dynamic coordinate
system modification and cutter compensation.
The scaling/rotation/polar coordinate does not support the G31 skip. Modify
the program.
The scaling/rotation/polar coordinate does not support skip operation.
The scaling/rotation/polar coordinate does not support the coordinate system
dynamic modification and cutter compensation.
Tool magazine does not use (fail to open the parameter). Tool-change
command M06 can not be used.
The scaling/rotation/polar coordinate does not support metic/inch input
APPEDIX
0220
This command can not be performed in G10 modal, it is better to cancel the
shifting.
Tool-chang macro program does not support the metic/inch input shifting.
Reference position return has not been performed before the automatic
operation starts.
Any of the following errors occurred in the specified format at the
programmable-parameter input:
0231
1) Address N or R was not entered;
2) Parameter number was not specified;
3) Address P in the bit-parameter input L50 does not specify;
4) N, P and R exceed its range. Modify the program.
0232
0233
Three or more axes were specified as the helical interpolation axes.
Other operations are being used the equipment connected with the
RS-232-C interface.
0235
The record end symbol (%) was specified.
0236
The parameter for specifying program restart is not set correctly.
0237
The command that should be specified the decimal point does not specify the
417
GSK218MC Series Machining Center CNC System Programming & Operation Manual
decimal point.
0238
The same address appears more than once in a block. Alternatively, a block
contains two ore more G codes belonging to the same group.
An illegal G code is specified at the pre-read control method; an index axis is
0239
specified in the pre-treat control method; the Max. cutting feed parameter
sets to 0; the parameter of acceleration/deceleration before interpolation sets
to 0. Correct the setting parameter.
0241
MPG pulse abnormality
0242
Bus connection error
0250
Axis name repeated. Modify the parameters No.: 175~179
0251
ESP alarm, after the alarm cancels, it is better to return the zero.
0252
Program illegal end (CNC transmission velocity is slow, reduce the feedrate)
0261
perform the zero return by resetting.
0262
DSP alarm DSP does not start; restart it again.
0263
DSP alarm DSP parameter setting error
0264
DSP alarm Delivery data are excessive big; restart it again.
0265
DSP alarm Disconnect with the bus, or fail to initialize the bus.
0266
0267
APPEDIX
0268
0269
0270
0271
The speed of DSP interpolation axis exceeds 200m/min.; Zero return is
performed again after controlling the reset button.
DSP initialization mark (5555) abnormality; Zero return is performed again
after controlling the reset button.
The output value of the DSP unit period pulse is excessive big; Zero return is
performed again after controlling the reset button.
DSP internal alarm; Zero return is performed again after controlling the reset
button.
That the DSP evenly divides the interpolation point length is excessive small.
That the DSP accepts the interpolation data is excessive small; zero return is
performed again after pressing the ESP.
0272
DSP receives the unidendified G code.
0273
DSP hardware data interchange abnormality (Command type)
0274
DSP hardware data interchange abnormality (Data type)
0275
The interpolation velocity multimplication is 0 in the high speed mode.
0280
Each axis should be set to 0 firstly when using the tool-setting function.
0281
418
DSP interpolation axis pulse command speed is excessive big, it is better to
Shift to the [SETTING] [TOOL-SETTING MIDDLE] interface when using the
tool-setting function.
0282
Check whether the tool setter is installed or set the bit parameter 1.6 to 1.
0283
Z axis exceeds the safety position, check the tool setter or tool length setting.
Appendix Two
Alarm List
0286
Automatic tool length measure error, perform it again.
0401
Drive alarm 01: Servo motor speed exceeds the setting value.
0402
Drive alarm 02: Main circuit power voltage excessive high
0403
Drive alarm 03: Main circuit power voltage excessive low
0404
Drive alarm 04: The numerical value of the position error counter exceeds the
setting value
0405
Drive alarm 05: Motor’s temperature is excessive high.
0406
Drive alarm 06: Speed regulator is saturation for a long time.
0407
Drive alarm 07: CCW, CW drive prohibition input are OFF.
0408
Drive alarm 08: The absolute value of the numerical value of the position
error counter exceeds 230.
Drive alarm 09: Encoder signal error
0410
Drive alarm 10: Control power ±15V is lower.
0411
Drive alarm 11: IPM intelligent module fault
0412
Drive alarm 12: Motor’s current excessive big
0413
Drive alarm 13: Servo drive and motor overloading (Instantaneously heat)
0414
Drive alarm 14: Brake circuit fault
0415
Drive alarm 15: Encoder counter abnormality
0420
Drive alarm 20: EEPROM error
0430
Drive alarm 30: Encoder Z pulse error
0431
Drive alarm 31: Encoder UVW signal error or unmatch with the encoder.
0432
Drive alarm 32: UVW signal exist full-high-level or full-low-level
0433
Drive alarm 33: Communication interruption
0434
Drive alarm 34: Encoder speed abnormality
0435
Drive alarm 35: Encoder state abnormality
0436
Drive alarm 36: Encoder count abnormality
0437
Drive alarm 37: Encoder single-loop count overflow
0438
Drive alarm 38: Encoder multi-loop count overflow
0439
Drive alarm 39: Encoder battery alarm
0440
Drive alarm 40: Encoder battery power-shortage
0441
Drive alarm 41: Unmatched motor type
0442
Drive alarm 42: Absolute position data abnormality alarm
0443
Drive alarm 43: Encoder EPPROM verification alarm
0449
Fail to initialize the Ethernet. Check the hardware
0450
Drive OFF, check whether the hardware is correctly connected.
0451
The 1st axis drive alarm
0452
The 2nd axis drive alarm
APPEDIX
0409
419
GSK218MC Series Machining Center CNC System Programming & Operation Manual
0453
The 3rd axis drive alarm
0454
The 4th axis drive alarm
0455
The 5th axis drive alarm
0456
Spindle drive alarm
0500
The 1st axis soft limit overtravel along -: (Manual or MPG releasing along +)
0501
The 1st axis soft limit overtravel along -: (Manual or MPG releasing along -)
0502
The 2nd axis soft limit overtravel along -: (Manual or MPG releasing along +)
0503
The 2nd axis soft limit overtravel along -: (Manual or MPG releasing along -)
0504
The 3rd axis soft limit overtravel along -: (Manual or MPG releasing along +)
0505
The 3rd axis soft limit overtravel along -: (Manual or MPG releasing along -)
0506
The 4th axis soft limit overtravel along -: (Manual or MPG releasing along +)
0507
The 4th axis soft limit overtravel along -: (Manual or MPG releasing along -)
0508
The 5th axis soft limit overtravel along -: (Manual or MPG releasing along +)
0509
The 5th axis soft limit overtravel along -: (Manual or MPG releasing along -)
0510
0511
0512
APPEDIX
0513
0514
0515
0516
0517
0518
0519
0600
420
The 1st axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along +)
The 1st axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along -)
The 2nd axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along +)
The 2nd axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along -)
The 3rd axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along +)
The 3rd axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along -)
The 4th axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along +)
The 4th axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along -)
The 5th axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along +)
The 5th axis hard limit overtravel along -: (Overtravel releasing, Manual or
MPG releasing along -)
Disconnect the operation keyboard. Check the operation keyboard
connection cable
1001
The address of relay or coil does not set.
1002
The function code of input code is absent.
Appendix Two
Alarm List
Function command COM does not use correctly, its corresponding
1003
relationship between COM and COME is incorrect, alternatively, the function
command is used between them.
1004
1005
1006
User ladder diagram exceeds the Max. allowable lines or steps.
(Troubleshooting) reduce the compiled NET numbers.
Function commands END1 and END2 are absent; or error in the END1 and
END2; or END1 and END2 are incorrect.
Illegal output in the network. Check the output format.
PLC is without communication due to the hardware fault or the system
1007
interruption error. It is necessary to contact the system equipment
manufacturer.
1008
Function code does not correctly connected.
1009
Fail to connect the network horizontal.
1010
1011
The network is being compiled is lost because the the power is turned off
while the ladder diagram is edited.
The address or data is inconsistent with the format of this function command.
Input again.
1012
The address or data does not correctly input. Input again.
1013
Illegal characters are specified or the data are exceeded its range.
1014
CTR address repeated. Select the unused CTR address again.
Function command JMP does not used correctly, the corresponding
relationships between JMP and LBL are incorrect. Alternatively, the JMP
APPEDIX
1015
function command is used again between JMP and LBL.
1016
1017
Incompleted network structure. Change the ladder diagram
The network structure does not support at present. Change the ladder
diagram.
1019
TMR address repeated. Select the unused TMR address again.
1020
The parameter is absent in function command. Input the legal parameter
PLC performance is overtime, the system will then stop the PLC
1021
automatically. Check the ladder diagram logic and eliminate the dead-cycle
or excessive repeated calling.
1022
Function command name is absent. Correctly input the function command
name.
1023
The address or constant of the function command exceeds its range.
1024
The unnecessary relay or coil exists. Delete the unwanted connection
1025
Function command correct output
1026
The line numbers of network connection are exceeded its support range.
Change the ladder diagram.
421
GSK218MC Series Machining Center CNC System Programming & Operation Manual
1027
The same output address is used in another position. Reselect the unused
the output address.
1028
Ladder diagram file format error
1029
The ladder diagram being used is lost.
1030
There is incorrect vertical line in the network. Delete the vertical line.
1031
1032
1033
User data area is already full, reduce the data table capacity of the COD
codes.
The 1st level of the ladder diagram is excessive big, which can not be
immediately performed it. Reduce the 1st level ladder diagram.
Function command SFT exceeds the Max. allowable use number. Reduce
the use amount.
1034
Function command DIFU/DIFD address repeated. Reselect the address.
1039
The command or network are not within the performable range. Clear it.
Fail to correcet use the function command CALL or SP; the corresponding
1040
relationships between the CALL and SP or the SP and SPE are incorrect.
Alternatively, either the SP function command is used again between the SP
and SPEC, or the SP is set before using the END2.
APPEDIX
422
1041
The horizontal breakover cable is parallel with the node network.
1042
Fail to load the PLC system parameter file.